<%BANNER%>

Finite Element Analysis for Use in Fluid Structure Interaction of a High Aspect Ratio Thin Airfoil using Drop-Plies

Permanent Link: http://ufdc.ufl.edu/UFE0041819/00001

Material Information

Title: Finite Element Analysis for Use in Fluid Structure Interaction of a High Aspect Ratio Thin Airfoil using Drop-Plies
Physical Description: 1 online resource (124 p.)
Language: english
Creator: Bonsmann, Jarrod
Publisher: University of Florida
Place of Publication: Gainesville, Fla.
Publication Date: 2010

Subjects

Subjects / Keywords: avl, fea, vic
Mechanical and Aerospace Engineering -- Dissertations, Academic -- UF
Genre: Mechanical Engineering thesis, M.S.
bibliography   ( marcgt )
theses   ( marcgt )
government publication (state, provincial, terriorial, dependent)   ( marcgt )
born-digital   ( sobekcm )
Electronic Thesis or Dissertation

Notes

Abstract: Abstract of Thesis Presented to the Graduate School of the University of Florida in Partial Fulfillment of the Requirements for the Degree of Master of Science FINITE ELEMENT ANALYSIS FOR USE IN FLUID STRUCTURE INTERACTION OF A HIGH ASPECT RATIO THIN AIRFOIL USING DROP-PLIES By Jarrod M Bonsmann May 2010 Chair: Peter Ifju Cochair: Bhavani Sankar Major: Mechanical Engineering One of the primary advantages in using fiber composite materials for mechanical applications is the ability of the user to tailor the mechanical properties of the material to its specific application. One such example is the use of graphite fiber woven cloth embedded in epoxy for the fabrication of high aspect ratio thin airfoils. These airfoils can be used in a number of fields from rotor blade technology to recreational and sporting equipment such as a racing windsurfing fin. This thesis uses a windsurfing fin for design verification. By using graphite/epoxy material one is able to vary the ply lay-up to produce different stiffness properties in the fin as well as different bend twist coupling characteristics in the airfoil. Mechanical tests using electrical resistance strain gages are performed to obtain the various material properties of the graphite/epoxy system used. ABAQUS finite element analysis (FEA) program and MatLab technical computing software are used to create a finite element model for use in analyzing the deformation characteristics of the fin in various loading conditions. The model deformations are verified using Visual Image Correlation (VIC) to study the deflections of a fin with known material lay-up properties and loading conditions. Once all of these tests and studies are performed Athena Vortex Lattice (AVL) program is used to obtain the fluid structure interaction pressure loads on a fin in water. With these loads and the computer model, a tool is developed that can be used to study and optimize the design of the windsurfing fin without the costly (both time and monetary) creation of a plethora of fins utilizing almost endless possibilities of ply lay-up directions and lengths.
General Note: In the series University of Florida Digital Collections.
General Note: Includes vita.
Bibliography: Includes bibliographical references.
Source of Description: Description based on online resource; title from PDF title page.
Source of Description: This bibliographic record is available under the Creative Commons CC0 public domain dedication. The University of Florida Libraries, as creator of this bibliographic record, has waived all rights to it worldwide under copyright law, including all related and neighboring rights, to the extent allowed by law.
Statement of Responsibility: by Jarrod Bonsmann.
Thesis: Thesis (M.S.)--University of Florida, 2010.
Local: Adviser: Ifju, Peter.
Local: Co-adviser: Sankar, Bhavani V.

Record Information

Source Institution: UFRGP
Rights Management: Applicable rights reserved.
Classification: lcc - LD1780 2010
System ID: UFE0041819:00001

Permanent Link: http://ufdc.ufl.edu/UFE0041819/00001

Material Information

Title: Finite Element Analysis for Use in Fluid Structure Interaction of a High Aspect Ratio Thin Airfoil using Drop-Plies
Physical Description: 1 online resource (124 p.)
Language: english
Creator: Bonsmann, Jarrod
Publisher: University of Florida
Place of Publication: Gainesville, Fla.
Publication Date: 2010

Subjects

Subjects / Keywords: avl, fea, vic
Mechanical and Aerospace Engineering -- Dissertations, Academic -- UF
Genre: Mechanical Engineering thesis, M.S.
bibliography   ( marcgt )
theses   ( marcgt )
government publication (state, provincial, terriorial, dependent)   ( marcgt )
born-digital   ( sobekcm )
Electronic Thesis or Dissertation

Notes

Abstract: Abstract of Thesis Presented to the Graduate School of the University of Florida in Partial Fulfillment of the Requirements for the Degree of Master of Science FINITE ELEMENT ANALYSIS FOR USE IN FLUID STRUCTURE INTERACTION OF A HIGH ASPECT RATIO THIN AIRFOIL USING DROP-PLIES By Jarrod M Bonsmann May 2010 Chair: Peter Ifju Cochair: Bhavani Sankar Major: Mechanical Engineering One of the primary advantages in using fiber composite materials for mechanical applications is the ability of the user to tailor the mechanical properties of the material to its specific application. One such example is the use of graphite fiber woven cloth embedded in epoxy for the fabrication of high aspect ratio thin airfoils. These airfoils can be used in a number of fields from rotor blade technology to recreational and sporting equipment such as a racing windsurfing fin. This thesis uses a windsurfing fin for design verification. By using graphite/epoxy material one is able to vary the ply lay-up to produce different stiffness properties in the fin as well as different bend twist coupling characteristics in the airfoil. Mechanical tests using electrical resistance strain gages are performed to obtain the various material properties of the graphite/epoxy system used. ABAQUS finite element analysis (FEA) program and MatLab technical computing software are used to create a finite element model for use in analyzing the deformation characteristics of the fin in various loading conditions. The model deformations are verified using Visual Image Correlation (VIC) to study the deflections of a fin with known material lay-up properties and loading conditions. Once all of these tests and studies are performed Athena Vortex Lattice (AVL) program is used to obtain the fluid structure interaction pressure loads on a fin in water. With these loads and the computer model, a tool is developed that can be used to study and optimize the design of the windsurfing fin without the costly (both time and monetary) creation of a plethora of fins utilizing almost endless possibilities of ply lay-up directions and lengths.
General Note: In the series University of Florida Digital Collections.
General Note: Includes vita.
Bibliography: Includes bibliographical references.
Source of Description: Description based on online resource; title from PDF title page.
Source of Description: This bibliographic record is available under the Creative Commons CC0 public domain dedication. The University of Florida Libraries, as creator of this bibliographic record, has waived all rights to it worldwide under copyright law, including all related and neighboring rights, to the extent allowed by law.
Statement of Responsibility: by Jarrod Bonsmann.
Thesis: Thesis (M.S.)--University of Florida, 2010.
Local: Adviser: Ifju, Peter.
Local: Co-adviser: Sankar, Bhavani V.

Record Information

Source Institution: UFRGP
Rights Management: Applicable rights reserved.
Classification: lcc - LD1780 2010
System ID: UFE0041819:00001


This item has the following downloads:


Full Text

PAGE 1

1 FINITE ELEMENT ANALYSIS FOR USE IN FLUID STRUCTURE INTERACTION OF A HIGH ASPECT RATIO THIN AIRFOIL USING DROP-PLIES By JARROD M BONSMANN A THESIS PRESENTED TO THE GRADUATE SCHOOL OF THE UNIVERSITY OF FLORIDA IN PARTIAL FULFILLMENT OF THE REQUIREMENTS FOR THE DEGREE OF MASTER OF SCIENCE UNIVERSITY OF FLORIDA 2010

PAGE 2

2 2010 JARROD BONSMANN

PAGE 3

3 To my Family, for always pushing me to become better at everything

PAGE 4

4 ACKNOWLEDGMENTS First and foremost, I would like to thank my advisor Professor Ifju for everything he has given and done for me over the two years of my stay at the University of Florida. His patience in dealing with the thousands of questions I had for him throughout the course of this research and advice were invaluable. Special thanks also goes out to Professor Sankar for all of his support in dealing with the finer aspects of creating an ultimate finite element model and serving as a co-advisor to me. I would also like to thank Professor Kumar for serving on my committee. Almost as valuable as any advice from my Professors was the advice given to me by my fellow graduate students and for that I thank Anurag, Vijay, and Weiqi for helping me learn about ABAQUS, Athena Vortex Lattice program, and mechanical testing respectively. Finally I would like to thank all my fellow lab mates in NEB 148. Without the fun that you guys have brought to my daily work life, I know I would never have made it half as far as I did.

PAGE 5

5 TABLE OF CONTENTS page ACKNOWLEDGMENTS .................................................................................................. 4 LIST OF TABLES ............................................................................................................ 8 LIST OF FIGURES .......................................................................................................... 9 LIST OF ABBREVIATIONS ........................................................................................... 13 ABSTRACT ................................................................................................................... 14 CHAPTER 1 INTRODUCTION .................................................................................................... 16 1.1 Composite Materials Used in Design ................................................................ 16 1.2 The Creation of a Windsurfing Fin .................................................................... 19 1.3 Research Objectives ......................................................................................... 21 2 MATERIAL PROPERTIES TESTING ..................................................................... 23 2.1 Strain Gages ..................................................................................................... 23 2.2 Tension Testing Background ............................................................................ 25 2.3 Tension Test Sample Preparation ..................................................................... 27 2.3.1 Specimen LayUp .................................................................................... 27 2.3.2 Machining the Tensile Test Specimen ..................................................... 29 2.3.3 Strain Gage Mounting .............................................................................. 29 2.4 The Tension Test .............................................................................................. 31 2.5 Shear Testing Background ............................................................................... 35 2.6 Shear Test Specimen Preparation .................................................................... 36 2.6.1 Machining the Shear Test Specimen ....................................................... 36 2.6.2 Shear Strain Gage Mounting ................................................................... 37 2.7 The Shear Test ................................................................................................ 38 3 THE DEVELOPMENT OF THE FINITE ELEMENT MODEL ................................... 43 3.1 Introduction to Finite Element Analysis ............................................................. 43 3.1.1 Background ............................................................................................. 43 3.1.2 Various Elements and their Strengths and Weaknesses ......................... 44 3.2 Initial Finite Element Models ............................................................................. 46 3.2.1 The Completely 20-Node Hexahedral Mesh ............................................ 47 3.2.2 The Completely 10-Node Tetrahedral Mesh ............................................ 48 3.3 Development of the Final Finite Element Model ............................................... 49 3.3.1 Important Characteristics of the New Finite Element Model .................... 50 3.3.2 Creation of an Input File Using MatLab ................................................... 50

PAGE 6

6 3.3.3 Shell Elements Utilized ............................................................................ 54 3.3.4 Solid Elements Utilized ............................................................................ 55 3.3.5 Element Set Interactions and Boundary Conditions ................................ 58 3.3.6 Automated Design Features of the Final Model ...................................... 60 4 VISUAL IMAGE CORRELATION ............................................................................ 63 4.1 Background Information .................................................................................... 63 4.2 Cantilever Point Load Test ................................................................................ 64 4.2.1 Sample Preparation ................................................................................. 64 4.2.2 Initial VIC Test SetUp ............................................................................. 65 4.2.3 Initial VIC Test ......................................................................................... 68 4.2.4 Modifications to Initial Test and Final VIC Test ........................................ 73 4.3 Twist Test Using VIC ........................................................................................ 75 4.3.1 Specimen Preparation ............................................................................. 76 4.3.2 Twist Test SetUp .................................................................................... 77 4.3.3 Twist Test Procedure ............................................................................... 78 5 RESULTS AND DISCUSSION ............................................................................... 80 5.1 Mechanical Properties Testing .......................................................................... 80 5.1.1 Tension Test Results ............................................................................... 80 5.1.2 Tension Test Discussion and Error ......................................................... 83 5.1.3 Shear Test Results .................................................................................. 85 5.1.4 Shear Test Discussion and Error ............................................................. 86 5. 2 VIC Results ....................................................................................................... 88 5.2.1 VIC Cantilevered Bending Test ............................................................... 88 5.2.2 VIC Twist Test ......................................................................................... 91 5.3 ABAQUS Results .............................................................................................. 93 5.3.1 ABAQUS Cantilevered Bending Test ...................................................... 93 5.3.2 ABAQUS Twist Test ................................................................................ 95 5.4 Matching the Data from ABAQUS and VIC ....................................................... 97 5.4.1 Matching the Bend Test Data .................................................................. 97 5.4.2 Matching the Twist Test Data ................................................................ 100 5.4.3 Matched Curves Discussion .................................................................. 105 6 ATHENA VORTEX LATTICE METHOD ............................................................... 107 6.1 Background Information .................................................................................. 107 6.2 Running AVL and Applying Loads to the Finite Element Model ...................... 108 6.2.1 Running AVL ......................................................................................... 108 6.2.2 Applying Loads to the Finite Element Model ......................................... 111 6.3 AVL Loading Condition Results and Discussion ............................................. 113 7 CONCLUSIONS AND FUTURE WORK ............................................................... 119 7.1 Conclusions .................................................................................................... 119 7.2 Future Work .................................................................................................... 120

PAGE 7

7 LIST OF REFERENCES ............................................................................................. 122 BIOGRAPHICAL SKETCH .......................................................................................... 124

PAGE 8

8 LIST OF TABLES Table page 3-1 Maximum deflections of the fin with the decreasing tetrahedron size ................. 49 5-1 Sample values for Poisson Ratio from first sample ............................................ 82 5-2 Sample values for Poisson Ratio from second sample ....................................... 83 5-3 Numerical results for maximum deflection of the fin at the six separate loading conditions ............................................................................................... 90 5-4 Numerical results for the maximum twist at the tip of the fin under a variety of torsion loading conditions ................................................................................... 92 5-5 Material Properties input into the final FEA code ................................................ 94 5-6 Equations of the fit lines and R-squared values for three loading conditions ...... 99 5-7 The fourth order polynomial and R-squared value of twist comparison for small loading case ............................................................................................ 103 5-8 Third order polynomial and R-squared values for bend data from small load twist test ........................................................................................................... 104 6-1 List of test data along with net force acting on the fin under each operating condition ........................................................................................................... 110 6-2 Net force experienced by NACA 0009 under given conditions ......................... 111 6-3 List of maximum deflections for given loading scenarios for 5 ply orientations ....................................................................................................... 116 6-4 Maximum deflections of 0/90 degree ply orientation at given loading scenarios .......................................................................................................... 117

PAGE 9

9 LIST OF FIGURES Figure page 1-1 Schematic illustrating the material coordinate system used in a bi-directional composite material (left) [1] and a piece of plain weave graphite cloth (right) .... 17 1-2 The equations used to define mid-plane deformation in a composite layup [2] ....................................................................................................................... 18 1-3 The equations defining members of the ABD matrix [2] ..................................... 18 1-4 Mold used to produce the windsurfing fin ........................................................... 19 1-5 Sc hematic illustrating concept of the drop-ply .................................................... 20 2-1 Picture of the linear strain gage (left) [5] from Omega used for tension testing and the shear strain gage from Micro-Measurements (right) [4] ......................... 25 2-2 Diagram showing Poisson effect in a sample under tension [7] ......................... 26 2-3 Typical stress strain curve from which Elastic Modulus may be determined [6] 27 2-4 Pictures showing the painting (left) and bubble busting (right) processes of the hand lay-up system ...................................................................................... 28 2-5 Il lustrating the mold once the plate is laid up and clamps applied ...................... 28 2-6 Picture of the tension test specimen once the strain gages are properly mounted ............................................................................................................. 31 2-7 Picture of the tension testing machine, the MTI-30K .......................................... 32 2-8 Diagram of the proper wire connection to the unidirectional tensile test [10] ...... 32 2-9 Diagram illustrating proper connection of strain gage wires to the NI SCXI 1321 [10] ............................................................................................................ 33 210 Picture showing the tension test specimen mounted into the testing machine ... 34 211 Diagram showing the proper dimension of an Iosipescu test specimen [12] ...... 35 212 Picture of the Iosipescu testing apparatus manufactured at the University of Florida ................................................................................................................ 37 213 Picture showing the properly machined specimen and mounted shear strain gages .................................................................................................................. 38 214 Schematic showing the proper wire hook up to the shear strain gage [10] ......... 40

PAGE 10

10 215 Schematic of the proper wire connections from strain gages to data acquisition box [10] ............................................................................................. 41 216 Picture showing the Iosipescu sample loaded into the testing fixture and into the MTI-30K ........................................................................................................ 42 3-1 Diagram showing nodal placement in a 20-node hexahedral element [13] ........ 45 3-2 Diagram showing node placement on a 10-node tetrahedron element [14] ....... 45 3-3 Deformation of fin using purely tetrahedron mesh under a point load ................ 48 3-4 Excel graph showing the thickness profile of the airfoil and the polynomial fit line ...................................................................................................................... 51 3-5 Excel graph displaying the leading and trailing edge profiles ............................. 52 3-6 ABAQUS rendering of the fin with only the shell elements created and each row of elements having own coordinate system ................................................. 55 3-7 Picture showing the width change in the solid elements at the termination of a drop-ply ........................................................................................................... 57 3-8 Picture showing each of the solid element sets with their respective material coordinate systems ............................................................................................. 57 3-9 Cross section of the final model illustrating all of the outer shells and the inner solid elements ............................................................................................ 60 310 ABAQUS rendering of the final Finite Element Model ........................................ 62 4-1 Speckle pattern on a portion of the fin ................................................................ 65 4-2 Picture showing the fin set-up for the initial VIC test .......................................... 67 4-3 Schematic of the VIC camera setup .................................................................. 68 4-4 VIC image of the calibration process .................................................................. 69 4-5 Image showing the application of the point load at the tip of the fin .................... 71 4-6 Graph showing deformation of fin in the initial VIC test ...................................... 72 4-7 Results of using a rectangular based fin and stronger clamping condition for the VIC bend test ................................................................................................ 75 4-8 Pro-Engineer rendering of the fin tip box ............................................................ 77 4-9 Fin set-up with torsion bar on tip of fin ................................................................ 78

PAGE 11

11 5-1 Stress Strain curve for aluminum sample ........................................................... 81 5-2 Stress-Strain plot of all three graphite/epoxy sample ......................................... 82 5-3 Graph showing data for shear modulus calculations for alumin um ..................... 85 5-4 Plot showing data for shear modulus calculations for all three Iosipescu samples .............................................................................................................. 86 5-5 Deformations in the z direction of the fin under a 2.5 pound point load at the tip ........................................................................................................................ 89 5-6 VIC W-Deformation vs. X-Position for three loading conditions (2.5, 6.5, and 11.8 pounds) ....................................................................................................... 89 5-7 Picture showing the deformation of the fin when 5.8 pounds are applied to the bar ...................................................................................................................... 91 5-8 VIC twist calculations for two separate loading conditions (5.8 and 8 pounds) .. 92 5-9 Medium load deformations as modeled in ABAQUS .......................................... 94 510 ABAQUS W-Deformation vs. X-Position for three separate loading conditions (2.5, 6.5, and 11.8 pounds) ................................................................................ 95 511 Schematic illustrating forces experienced by the fin under twist load ................. 96 512 ABAQUS deformations under large applied torque ............................................ 96 513 ABAQUS Twist deformation curves for two separate loading conditions (5.8 and 8 pounds) ..................................................................................................... 97 514 Deflection curves comparison for three loading conditions ................................ 99 515 Plot showing the leading and trailing edge profiles obtained from ABAQUS and the VIC data ............................................................................................... 101 516 Plot showing twist deformation comparison for two loading conditions ............ 102 517 Bend data comparison from the two separate loads twist tests ........................ 104 6-1 MatLab graph rendering the fin surface input into the AVL program ................ 112 6-2 ABAQUS rendering of the forces from AVL applied to the final finite element model ................................................................................................................ 113 6-3 W-deflection of fin traveling 20 knots with one degree AOA and 5 degree ply orientation ................................................................................................... 114

PAGE 12

12 6-4 Deflection curves for 10 knot speed and different angles of attack and ply orientation ......................................................................................................... 115 6-5 Deflection curves for 20 knot speed and different angles of attack and ply orientation ......................................................................................................... 115 6-6 Deflection curves for 30 knot speed and different angles of attack and ply orientation ......................................................................................................... 116

PAGE 13

13 LIST OF ABBREVIATIONS AOA Angle of Attack C L Coefficient of Lift DIC Digital Image Correlation FEA Finite Element Analysis VIC Visual Image Correlation

PAGE 14

14 Abstract of Thesis Presented to the Graduate School of the University of Florida in Partial Fulfillment of the Requirements for the Degree of Master of Science FINITE ELEMENT ANALYSIS FOR USE IN FLUID STRUCTURE INTERACTION OF A HIGH ASPECT RATIO THIN AIRFOIL USING DROP-PLIES By Jarrod M Bonsmann May 2010 Chair: Peter Ifju Cochair: Bhavani Sankar Major: Mechanical Engineering One of the primary advantages in using fiber composite materials for mechanical applications is the ability of the user to tailor the mechanical properties of the material to its specific application. One such example is the use of graphite fiber woven cloth embedded in epoxy for the fabrication of high aspect ratio thin airfoils. These airfoils can be used in a number of fields from rotor blade technology to recreational and sporting equipment such as a racing windsurfing fin. This thesis uses a windsurfing fin for design verification. By using graphite/epoxy material one is able to vary the ply layup to produce different stiffness properties in the fin as well as different bend twist coupling characteristics in the airfoil. Mechanical tests using electrical resistance strain gages are performed to obtain the various material properties of the graphite/epoxy system used. ABAQUS finite element analysis (FEA) program and M at L ab technical computing software are used to create a finite element model for use in analyzing the deformation characteristics of the fin in various loading conditions. The model deformations are verified using Visual Image Correlation (VIC) to study the deflections of a fin with known material lay-up properties and loading conditions. Once all of these

PAGE 15

15 tests and studies are performed Athena Vortex Lattice (AVL) program is used to obtain the fluid structure interaction pressure loads on a fin in water. With these loads and the computer model, a tool is developed that can be used to study and optimize the design of the windsurfing fin without the costly (both time and monetary) creation of a plethora of fins utilizing almost endless possibilities of ply lay-up directions and lengths.

PAGE 16

16 CHAPTER 1 INTRODUCTION This paper focuses on the development and verification of a finite element model for use in the design of a high aspect ratio thin airfoil in the form of a windsurfing fin. Such a model can easily be developed for isotropic materials, but when considering a fin created from a woven graphite fabric embedded in an epoxy matrix, the model becomes much more complex. Adding to the complexity of the model is the use of drop-plies in the creation of the fin that allows the thickness of the fin to be tapered down from the root to the tip. In order to develop a design tool for the creation of the optimum fin, the various nuances of a fibrous composite material must be understood. By creating a model as a design tool, various inputs including fiber angle, ply length, and fiber/matrix material can be varied in a computer simulation in order to study the deformation characteristics of specific fin designs without actually going through the process of creating multitudes of expensive fins. Though the research of this paper is directed towards the recreational field of windsurfing, the applicability of such research extends far beyond to fields such as rotor blade, wing, and numerous other high performance part designs. 1.1 Composite Materials Used in Design When designing any object that will be subjected to loads and undergo specific deformations it is important to understand the material with which the object will be made. The use of graphite/epoxy for design holds many advantages over traditional manufacturing materials. One of the primary advantages for the previously stated application is the ability to vary the stiffness and bend/twist characteristics of the fin by orienting the cloth in different directions. Figure 1-1 shows a schematic of a typical cloth

PAGE 17

17 that will be embedded in a matrix material, in this case epoxy. As seen in Figure 1-1 composite materials use a different coordinate system when associating applied stresses and resultant strains to the stresses and strains in the material. The warp and fill directions are the directions of the fibers, oriented at 90 degrees with respect to one another. The third direction is the out of plane direction. Figure 1-1: Schematic illustrating the material coordinate system used in a bidirectional composite material (left) [1] and a piece of plain weave graphite cloth (right) The mechanical properties of a woven cloth composite material differ greatly from that of an isotropic material. The in-plane (warp and fill) stiffness characteristics are dominated by the fiber material whereas the outof -plane properties will be indicative of the matrix material. As such, when designing with composite materials it is important that one realizes that an object made with the fibers oriented at 5 degrees with respect to the horizontal will have vastly different properties (with respect to a Cartesian coordinate system) than that of the same geometry object made with the fibers oriented in the 0 and 90 degree directions. Another interesting nuance of designing with composite materials comes as the bend/twist coupling characteristics of a lay-up. The stresses and strains in the global

PAGE 18

18 Cartesian coordinate system are related by the material ABD matrix shown in Figure 1-2 and Figure 1-3. Figure 1-2: The equations used to define mid-plane deformation in a composite layup [2] Figure 1-3: The equations defining members of the ABD matrix [2] The relations shown in the preceding figures have the potential to give rise to some interesting mechanical behavior if the manufactured object has a specific ply lay-up. Depending on the symmetry and angles of orientation of the different layers in the processed object, there is the potential to create bend/twist coupling in a material. This is a useful tool for creating a fin or wing that takes advantage of the principle of washout.

PAGE 19

19 1.2 The Creation of a Windsurfing Fin It is necessary now to understand how the windsurfing fin in consideration is manufactured. As stated before, the fin was made using a graphite fiber woven cloth specifically a 6k (6000 fibers per yarn) plain weave cloth, cured into the West Systems 105 Resin System using the 205 Fast Hardener. The hand layup compression molding method was used to create the fin. Initially, templates were used to cut out pieces of graphite epoxy cloth in various shapes and sizes used to fill the mold. The epoxy was then mixed using dispenser pumps to ensure proper mix ratios. A symmetric mold (two pieces with half of the geometry cut into each side) as seen in Figure 14 was used to shape the graphite/epoxy material. Figure 1-4: Mold used to produce the windsurfing fin The first layers were placed one onto each side of the mold and the epoxy spread over them using a simple paint brush. A bubble buster (serrated roller) was then utilized to eliminate bubbles from the surface of the cloth to prevent such occurrences from turning

PAGE 20

20 into voids in the fin once the epoxy cured. Another layer spanning the entire mold cavity was then placed over each of the previous layers and epoxy once again spread and bubbles eliminated. Once the outermost two layers on each side were laid the first drop-plies were created. The geometry of the fin is such that the same airfoil shape is maintained throughout the length of the fin. However, the thickness at the tip is only a fraction of the thickness at the root; since the fins chord decreases so too must the thickness. Droppl ies make this possible. A drop-ply is simply a piece of the cloth that is cut shorter than the length of the fin so that when placed starting at the root the piece of graphite cloth will terminate before the tip of the mold (as seen in Figure 15) Figure 1-5: Schematic illustrating concept of the drop-ply By using various lengths of drop-plies and proceeding with the same hand layup method, the rest of the mold was filled so that the cavity in the mold is even with the surrounding flat mold surface. Once filled, the two mold halves were placed together and aligned using pins fit through symmetrically drilled holes in both sides of the mold. C-clamps were then used to provide even pressure distribution on the mold to squeeze out excess epoxy and further eliminate voids. The mold was then left to allow the epoxy to cure and harden for at least 6 hours before demolding, but was not used for 24 hours so as to allow the

PAGE 21

21 epoxy to cure to maximum strength. Once removed from the mold the fin s surfaces were sanded down to a smooth finish with a sharp trailing edge. 1.3 Research Objectives The knowledge of the mechanics of materials of a composite system and an understanding of the production method used to manufacture a windsurfing fin is a necessary precursor to the research presented in this paper. The process of creating a single graphite/epoxy windsurfing fin costs the producer around 100 dollars. As such, the brute force method of creating innumerable fins for determining exactly what fiber orientation, drop-ply length, and fiber material to use for the best performance is neither economical nor appealing. To this end a finite element model was produced to exactly portray the deformation tendencies of a windsurfing fin produced in the manner stated above. In order to create such a model, the material properties of the graphite/epoxy system were determined through mechanical testing. Once these properties were determined and the model developed, it was experimentally verified. To prove the validity of said model, visual image correlation (VIC) testing was implemented through two different loading mechanisms to compare both the bending and the twisting of the actual fin to that of the computer model. The final objective of this research was to study how the fin will deform under realistic loading conditions. With a verified model, the geometry of the fin can be used in a hydrodynamic analysis program to get the loads experienced during actual use. With these loads and the ability to change material property, ply angle, and ply-drop-off length in the model an effective design tool was developed to create the optimal

PAGE 22

22 performing fin. This research is also applicable to various other areas such as composite rotor blade technology.

PAGE 23

23 CHAPTER 2 MATERIAL PROPERTIES TESTING One of the first steps in the design of any mechanical apparatus is to understand the material that the object will be made of. Design with aluminum differs from design with wood which differs from design with other materials such as the graphite/epoxy from which the windsurfing fin in consideration was manufactured. For the research in this paper it was necessary to obtain the various material properties that will be responsible for dictating the deformation characteristics of the entire fin. In order to get the physical properties of the material, electrical resistance strain gages were utilized in tensile and shear deformation tests. 2.1 Strain Gages One of the most readily available and fundamental methods for measuring strain in a material is the electrical resistance strain gage. The strain gage is based on the concept that a thin metal folded wire will change its length, cross sectional area, and electrical resistance once placed in a carrier material, bonded onto a surface, and strained. The changes in the above three things, through a series of algebraic relations and substitutions allows for the strain to be calculated in a material by sensing the change in voltage across the resistor (gage). Important considerations when dealing with strain measurements using electrical resistance strain gages include some of the following [3]: 1. The ability to precisely measure strain in static or dynamic situations 2. Independence of the influence of temperature 3. Stability of calibration 4. Linear response to strain For this research all four of these considerations were of paramount importance. For the tension and shear testing it was necessary to measure the strain as the material

PAGE 24

24 was loaded giving a precise correlation between the force applied to and the strain experienced by the specimen. Independence to temperature was an important consideration when dealing with gages operating as fluctuating heating or cooling conditions. The tests involving strain gages were performed in a laboratory setting that is subject to temperature differences of 3 degrees Fahrenheit. As such, it was important that the gage be relatively unresponsive to such temperature changes so as to not give false readings of strain. Calibration stability and linearity of the strain response were both important when dealing with the actual strain readings developed from the instrumentation. For this research, two different types of strain gages were used for the two different tests performed. For the tensile tests, the SGD-4/120-LY11 linear strain gage was used. This is a 120 ohm resistance strain gage with a 1.99 gage factor and a tolerance of .35%. Important considerations for choosing this gage were that the wires were all oriented in one direction for linear strain measurement along the orientation of the wire. For the measurement of shear strain the N2AXX -C032A500/SP61 by Micro-Measurements group is used. These strain gages can be viewed in Figure 2-1. This gage was specifically designed for the measurement of shear strains in Iosipescu samples. Strain responses in these samples are oftentimes non-linear so the gage must be able to This is done by placing the gage over the entire area of interest, namely between the notch in the Iosipescu sample [4].

PAGE 25

25 Figure 2-1: Picture of the linear strain gage (left) [5] from Omega used for tension testing and the shear strain gage from Micro-Measurements (right) [4] 2.2 Tension Testing Background One of the most basic tests that can be performed on a material to produce information about the mechanical properties of that coupon is the uniaxial tension test. The uniaxial tension test is simply a test where a sample of a material is mounted in a testing fixture and axially loaded in tension. While being loaded, the sample tends to elongate in the direction of loading and contract in the transverse direction. Measurement of the strain in the direction of the load and knowledge of the applied force from the machine and the test cross-sectional area of the sample leads to the development of a stress-strain curve specific to every material. Once a stress-strain curve is developed it is possible to determine the Modulus of Elasticity of the sample material. Another useful feature of the tension test is the ability of the test to produce results leading to the determination of the Poisson ratio of the material. By placing a second strain gage perpendicular to the gage along the loading axis, the contraction of the material in the transverse direction due to the elongation in the testing direction can

PAGE 26

26 be measured. Once this value is known, a simple ratio is taken to determine the Poisson ratio. A schematic illustrating this effect can be seen in Figure 22. (Equation 1) Figure 2-2: Diagram showing Poisson effect in a sample under tension [7] In the materials testing of the graphite/epoxy composite used in this research the tension test was extremely important. One tension test can be responsible for giving the information needed to determine three different material properties. If the gages are oriented along the warp and fill direction of the composite and loaded in the warp direction the strain in the warp and fill (1 and 2) directions can be found. Once the stress-strain curves in the 1 and 2 directions are developed the Modulus of Elasticity in each of these directions (E 1 and E 2 ) can be found by taking the slope of the linear portion of the curve. Using the relation in Equation 1 the Poisson Ratio in the 12 12 ) can also be determined. An example of a typical stress-strain curve is shown in Figure 2.3.

PAGE 27

27 Figure 2-3: Typical stress strain curve from which Elastic Modulus may be determined [6] 2.3 Tension Test Sample Preparation 2.3.1 Specimen LayUp The first step in the tension test process was the actual creation of the specimens In order to correctly characterize the windsurfing fin under scrutiny, the same material and lay-up process must be used in the creation of the test specimen that was used to create the fin. For this experiment the same 6k plain weave graphite cloth was used in the West Systems 105 Resin System with the 205 Fast Hardener. The hand layup described in the production section of this paper was also used. Instead of a two sided fin shaped cavity mold, two plates made of Teflon plastic acted as the mold. Four sheets measuring eight inches in length and width were cut out of the larger roll of graphite fiber cloth. The first layer of cloth was laid upon the plate, brushed with epoxy and bubble busted (see Figure 24) The same process was repeated for the next three layers.

PAGE 28

28 Figure 2-4: Pictures showing the painting (left) and bubble busting (right) processes of the hand lay-up system Once all of the layers were laid onto the bottom plate, the top Teflon plate was placed over the bottom Teflon plate containing the graphite/epoxy sheet and clamped as shown in Figure 25, using C-clamps for evenly distributed pressure. The mold was left for 24 hours as stated on the West Systems Hardener in order to allow the epoxy ample time to cure to maximum strength. Figure 2-5: Illustrating the mold once the plate is laid up and clamps applied After the time for curing elapsed, the mold was taken apart and the graphite/epoxy plate separated from the mold.

PAGE 29

29 2.3.2 Machining the Tensile Test Specimen Using the compression mold hand lay-up method described, an 8x8 inch sheet was produced. A diamond tile saw was used to cut the outer three quarters of an inch off of each side to create a 6.5x6.5 inch plate. The reason for cutting the outside edge off of the plate was to get rid of any part of the plate that does not have the fibers distributed uniformly throughout. During the lay-up, when bubble busting, the yarns of fibers tend to get pushed around and towards the edges, can sometimes fray and become discontinuous. By cutting the edges these parts were eliminated. After the smaller area plate was made, strips slightly wider than a half of an inch were cut from the material. It was an important consideration to make sure that the strips are cut so that the length and width of each strip line up perfectly with the fibers in the warp and f ill direction. These strips were then placed in a straight edge clamping device and sanded down to a half of an inch width. The reason the straight edge clamping device was employed is to make sure that the sides of each test strip are straight parallel lines. After the tension test samples were physically prepared, they must be outfitted for the actual test. Initially, grip tabs were placed on both ends of the test specimen and bonded there using epoxy. These tabs were necessary because the grips used in the tension test machine need ed a material to clamp down-on and in-to in order to stop the grips from slipping, resulting in erroneous readings. 2.3.3 Strain Gage Mounting The strain gage configuration on the specimen was two strain gages on each side of the sample, one mounted along the axis of loading, and the other placed transverse to the first. Strain gages were mounted on each side opposite one another to account for any bending in the specimen during the test; i.e. the negative compression reading

PAGE 30

30 due to bending on one side of the specimen will cancel out the positive bending tension reading on the other. The strain gages were mounted using the following guidelines illustrated in the Vishay Micro-Measurements strain gage bonding manual [8]: 1. The surface of the specimen was degreased using CSM-1A degreaser and a clean cotton swab. 2. The surface was then coated with M-Prep Conditioner, and lightly abraded using a 400 grit sand paper to remove any loosely bonded surface adherents. 3. After abrasion another clean cotton swab was used to dry the surface making sure to not drag any contaminates into the gage area 4. Layout lines we re drawn on the specimen. Two lines were drawn; one along the loading axis and one perpendicular to it. If the specimen is machined properly the lines will correspond to the fiber directions in the specimen. 5. M-Prep Conditioner was applied once more to the surface and a Q-Tip was used to scrub the layout line area until the tip comes away clean. The surface was then wiped using another clean cotton swab. 6. M-Prep Neutralizer was then put on the surface and scrubbed with another Q-Tip to provide the correct surface alkalinity for the optimum bond. It was once again wiped clean with another swab. 7. The strain gage was stuck to a piece of M-Line PCT-2A cellophane tape and using an optical microscope the gages were placed so that the arrows on the gage line up with the previously marked layout lines. 8. The tape was peeled up until just after the strain gage was lifted off of the surface and M-Bond 200 Catalyst was applied sparingly to the bottom surface of the strain gage. 9. After waiting one minute for the Catalyst to dry a drop of M-Bond 200 Adhesive was applied to the area directly in front of the strain gage. 10. The tape was then placed down in a smooth motion and held for two minutes to allow time for the adhesive to dry. 11. The tape was peeled up and the strain gage successfully bonded. After the strain gages were mounted, the lead wires from the strain gage were attached to the soldering tabs. This was accomplished obviously by laying a bead of

PAGE 31

31 solder on the tabs and soldering the wire to the tab. A picture of one of the tension test specimens with strain gages mounted to the surface can be seen in Figure 26. Figure 2-6: Picture of the tension test specimen once the strain gages are properly mounted 2.4 The Tension Test After the entire sample preparation was performed, the tensile test commenced. The first step in the tension test process was the careful placement of the specimen into the grips used by the tension test machine. The grips were aligned with the edges of the specimen which should also line them up with the fiber direction as well as the direction of the strain gage used to measure axial strain. Once that was accomplished the grips were tightened using an allen wrench, making sure no stress was placed on the specimen during the process. Once the grips were applied and tightened, they were fitted into the testing apparatus using a pair of clevis pins. The testing machine used was the MTI-30K system manufactured by Measurements Technology Inc. The MTI30K seen in Figure 27, is a testing system that can be used in either tension or compression. It has a 33,750 pounds force load

PAGE 32

32 capacity and the loading speed ranges from 0.0025 mm (0.0001 inches) to 250 mm (10 inches) per minute [9]. Figure 2-7: Picture of the tension testing machine, the MTI-30K After the sample was installed into the MTI-30K, rubber insulated wires were attached to the soldering tabs (and by proxy the lead wires of the strain gage) by using the soldering iron and re-melting the solder already on the tabs and connecting the wire. These wires were subsequently connected to a National Instruments SCXI-1321 data acquisition box. Diagrams illustrating the correct connections are shown in Figure 28 and Figure 2-9. Figure 2-8: Diagram of the proper wire connection to the unidirectional tensile test [10]

PAGE 33

33 In Figure 2-9 a resistor is seen to be placed in two outlets for each strain gage. This is a dummy resistor used to complete the strain gage circuit. The tension test strain gages were used in the quarter bridge configuration. In order to complete the circuit and have the ability to receive proper strain measurements a dummy resistance must be added. For this experiment, a 120 ohm resistor was chosen to match the resistance value of the strain gage. Figure 2-9: Diagram illustrating proper connection of strain gage wires to the NI SCXI 1321 [10] Now that the sample was properly secured in the testing machine as seen in Figure 210 and the strain gages were connected to the data acquisition box, the strain gages were calibrated using the National Instruments LabView program. Once the gages were properly calibrated, a load was applied to the sample via the MTI-30K. A 1000 pound force load cell was used to output the load applied. The load cell output was checked and calibrated by hanging a series of known weights from the load cell

PAGE 34

34 and cross checking the LabView load readout. Once calibrated, the load w as applied to the sample. Figure 2-10: Picture showing the tension test specimen mounted into the testing machine At each load the LabView program was setup to record the corresponding strain and output the data to a spreadsheet. The sample was not loaded until failure; rather it was only applied in the elastic range of the material. This was done because the test was performed to receive material properties E 1 E 2 12 none of which require data beyond that of the elastic stress-strain. Once the data was all acquired, the load from the machine was reversed and removed. The clevis pins were taken out and the sample was unloaded from the grips. This process was repeated for three different samples in order to verify the results Further verification was achieved by mounting the same type of strain gage on a piece of aluminum and calculating the Modulus of Elasticity for that known and well documented material. The results of these tests appear in Chapter 5.

PAGE 35

35 2.5 Shear Testing Background Another material property that was obtained through mechanical testing was G 12 the shear modulus in the 1-2 direction. Although a number of methods have been developed including the off-axis tension test, the Iosipescu test was the one chosen for this research. The Iosipescu test was originally developed as a test for determining shear modulus in metals [11]. Since that time the test has been adapted and reformed to accommodate specimens made from composite materials. The Iosipescu test was designed to create a state of pure shear at a certain cross section of a specially prepared specimen. In order to accomplish this, the specimen geometry must be different from that of the geometry of the specimen described for the uniaxial tension test as can be seen in Figure 211 configuration has the advantage that it is compact requiring small amounts of material, the instrumentation Figure 2-11: Diagram showing the proper dimension of an Iosipescu test specimen [12] As seen in the previous figure, the specimen must be created with notches in the middle. The testing apparatus was traditionally designed to put one side in tension in the upward direction (if the specimen is oriented as seen in the preceding figure) and put the opposite side in downward tension. By creating this loading condition, the

PAGE 36

36 notched portion of the Iosipescu specimen is put into a state very close to pure shear. One of the reasons the Iosipescu test was chosen for this research because knowledge of other graphite/epoxy material properties was not needed in order to determine G 12 ; as opposed to the off axis tension tests which requires the elastic modulus to be known for the determination of the shear modulus. 2.6 Shear Test Specimen Preparation The initial stages of the Iosipescu test sample preparation were the exact same as those used in that of the tension test. The composite plate was produced in the same hand lay-up fashion. The differences in the preparation stages will be shown here. 2.6.1 Machining the Shear Test Specimen Similar steps were taken in the production of the shear test specimen as were taken for the tension test specimen. Out of the initially formed graphite/epoxy plate, small strips were cut with dimensions slightly larger than 76.2x19.1 millimeters. To cut these strips the same diamond saw blade in the tile saw was used. As with the tension test specimen, special care was taken to cut the samples so that the fibers were lined up with the horizontal and longitudinal edges. The purpose of this test was to determine the shear modulus in the 12 direction, and the test works only if the specimen was able to be loaded properly. To apply this load the apparatus shown in Figure 212 was employed. Once the strips are cut, again the rough samples were placed into the straight edged clamping device so that the samples could be sanded down to the exact 76.2x19.1 millimeter dimensions. Both the width and length dimensions were of particular importance in this experiment. The load transmitting apparatus has slots in it that were machined to the dimensions necessary to: 1. Position the sample so that the strain gage is in the center of the transverse load

PAGE 37

37 2. Keep the sample from slipping in the grips by means of reaction force on the sample provided from the apparatus walls Figure 2-12: Picture of the Iosipescu testing apparatus manufactured at the University of Florida With the sample in the shape of a rectangle with the specified dimensions, the notches were made. To achieve an arc of specified radius at the tip of the notch, a 1.3 millimeter radius diamond tipped drill bit was used in a milling machine to drill two holes 14.1 millimeters apart, creating the notch radius required for the test. Once the holes were drilled, a Dremel tool was used with circular diamond blades to cut out the notch on either side of the sample. Unlike the tension test specimen, it was unnecessary to install grip tabs on the ends of the Iosipescu sample. The testing apparatus does not employ toothed grips that dig into the sample, making such grip tabs obsolete. 2.6.2 Shear Strain Gage Mounting Much care was taken when mounting the strain gages on Iosipescu specimen. As stated in the introduction to the shear strain gage, the shear strain developed during the shear test is a non-uniform field. Because of this fact, the strain gage, when mounted, must cover the entire area between the two notches machined in the previous step in order to average the strain field properly. Two strain gages were mounted-one on each

PAGE 38

38 side of the sample. The same logic drives the doubly mounted strain gages in this experiment as it d id with the tension test. The length of the strain gage is controlled by the production company, and should exactly match the length of the material lying between the two notches on the specimen. Referring to Figure 2-1, the gage was oriented so that the wires were perpendicular to a line drawn between the two notches, and the line separating the two sides of folded wire in the gage lined up exactly with the same line. A properly mounted gage onto an Iosipescu sample can be viewed in Figure 2-1 3. The specific mounting instructions given in the tension test section were also followed for the shear test. The surfaced was cleaned, conditioned, abraded, conditioned, and neutralized. The gages were aligned, treated with catalyst, and bonded to the surface with the adhesive. After the strain gages were mounted and bonded, the lead wires in the gage were soldered to a solder tab. Figure 2-13: Picture showing the properly machined specimen and mounted shear strain gages Following all of these instructions, the strain gages were perfectly mounted to the Iosipescu samples. 2.7 The Shear Test Once the strain gages were mounted, the Iosipescu test was performed. The first requirement was to place the sample into the Iosipescu test fixture. As described in the introduction to the shear test section, the Iosipescu test fixture is basically two pieces

PAGE 39

39 manufactured to provide tension on one side of the specimen notch in the upward direction and downward tension on the other side of the notch. There is a single slot in each of the two sides of the test fixture where the end of each sample can be placed and clamped down on by use of tightening four screws. When mounting the specimen into the fixture, the primary concern was the sample placement. Care was taken to position the sample so that the area where the strain gages were bonded was in the exact center between the two pieces of the test fixture. The test specimen was also checked to make sure that there was no twist once mounted, namely that the horizontal ends remain ed horizontal with respect to the testing fixture and the vertical ends remain ed vertical. After the sample was mounted in the test fixture, the fixture needed to be connected to the testing machine. The same testing machine, the MTI-30K, was used for this experiment. To connect the Iosipescu testing fixture to the MTI-30K clevis pins were once again utilized. In order to properly place the fixture in the machine, the clevis pins were slid through the Iosipescu fixture and the ma properly mounted, the tension test rods hooked up to the load cell and bottom of the test machine should make a perfect unbroken line with the two clevis pins hooked through the fixture and the notched portion of the sample. The next step in the testing preparation was the connection of the strain gages to the computer instrumentation. As with the tension test, the Iosipescu test uses a National Instruments SCXI-1321 data acquisition device coupled with the LabView program. Insulated wires were connected via soldering to the strain gages in a manner shown in Figure 214. The wires were taped to the Iosipescu testing fixture to prevent

PAGE 40

40 violent motion that could potentially snap the soldering tabs and lead wires off of the strain gage. Figure 2-14: Schematic showing the proper wire hook up to the shear strain gage [10] It was important to connect the wiring on the strain gage as shown in Figure 214 in order to achieve accurate strain readings. Once the wires were soldered to the strain gage lead wires, they were connected to a SCXI Terminal box. The shear strain gage was used as a half bridge circuit configuration, as opposed to the quarter bridge configuration of the tension test. It can be seen in Figure 2-15 that there is no external dummy resistance required to complete the strain gage circuit and receive accurate strain measurements.

PAGE 41

41 Figure 2-15: Schematic of the proper wire connections from strain gages to data acquisition box [10] After careful preparation the test was performed with the sample loaded in the testing machine as shown in Figure 216. In the same manner as the tension test, a load was applied to the specimen from the load cell transmitted into pure shear by the test fixture and specimen geometry. At each loading condition strain measurements were taken and written to a spreadsheet. The specimen was not loaded to failure but only loaded in what was expected to be the linear elastic range. This linear elastic data later provided the information needed to compute the shear modulus G 12 for which this test was performed.

PAGE 42

42 Figure 2-16: Picture showing the Iosipescu sample loaded into the testing fixture and into the MTI-30K Once all of the test data was acquired, the load was reversed and removed from the specimen, the fixture was unloaded from the machine, and the sample removed. Three separate samples of graphite/epoxy were tested in shear. This concludes the materials testing portion of the research, the results of which can be viewed in Chapter 5.

PAGE 43

43 CHAPTER 3 THE DEVELOPMENT OF THE FINITE ELEMENT MODEL The next and possibly the most challenging portion of the research was the development of the finite element model. A computer model that accurately portrays the mechanical response of the fin under realistic loads was the ultimate goal of the research. Though all aspects of the research were critical to accomplishing this goal, the model was perhaps paramount among them. For this reason this chapter will go more in depth than the others illustrating the various approaches used and stating why certain approaches failed where ultimately the final finite element model succeeds. 3.1 Introduction to Finite Element Analysis 3.1.1 Background A finite element analysis (FEA) program is computer software that uses numerical methods to solve several differential equations specific to certain problems. For example, if a truss structure is being designed for a building and the engineer wishes to quickly determine the stresses and strains that will be experienced in each web, two predominant solution methods are generally prescribed. The first is the analytical solution to the problem which involves a solution developed by hand using the characteristic equations for the situation. The second solution lies in the application of finite element software that, with minimal training, almost anyone can operate. The simplest solution to such a problem is obvious ly developed using FEA programs. This becomes more true when dealing with problems that do not have as clear and concise solution as those that involve, as an example, beams in simple bending. Although simple problems often do not require any more than the most basic model, more complex models are necessary for those problems involving:

PAGE 44

44 1. Complex geometries 2. Advanced structure interactions 3. Difficult materials in terms of complicated material properties For the research presented in this paper, all three of the preceding intricacies were involved in the development of the model. For the creation of the more in depth finite element model, a further knowledge of the inner workings of the FEA program, and the assumptions off of which these working are based, is necessary. As such, some of the base knowledge will be presented here. 3.1.2 Various Elements and their Strengths and Weaknesses An extremely general analysis of how FEA programs function follows. There are a number of elements in the repertoire of a finite element program. Each of these elements have characteristic equations governing how each will react to specific stress conditions, whether these conditions are due to mechanical, thermal, or acoustical loading among many other load forms. These elements have nodes at different positions and the governing equations are solved for each element to calculate the stresses or displacements at each node. A few examples of elements that can be used to solve an engineering problem in a finite element program, and the elements that were used in this research are; the shell element, the 20-node hexahedral (hex) element, and the 10-node tetrahedron element. The 20-node hexahedral element, also called the 20-node brick, is basically a rectangular cubic structure with nodes on each corner, and at the midpoint of each edge as shown in Figure 31. This element is one of the most accurate elements available in most commercial FEA programs. It is a quadratic element, meaning that non-linear strain is calculated through the element. The downfall of the 20-node brick element is the computational power involved in processing a model modeled exclusively with these

PAGE 45

45 elements. Since there are 20 nodes in each of these elements, if a structure is modeled with 100 elements then it is necessary for the computer to solve differential equations for two thousand nodes. Since computational time adds up significantly in complex models the use of 20-node brick elements should be saved for when they are most needed. Figure 3-1: Diagram showing nodal placement in a 20-node hexahedral element [13] The 10-node tetrahedron element is a second order triangular element. It, as with the 20-node hex element, has a node on each corner and the midpoint of every edge (see Figure 32) The first order tetrahedron element assumes constant strain through the element, making it a poor choice for any element involved in tests where large bending or twisting deformations occur. The second order tetrahedron does a better job, being a quadratic element, but still does not as accurately capture deformation as a 20-node hexahedral element. Figure 3-2: Diagram showing node placement on a 10-node tetrahedron element [14]

PAGE 46

46 -walled structures where bending and inelement acts like a 2-D beam with a thickness associated to it. The shell is a set of eight nodes in a roughly rectangular shape. There are four nodes on each corner and four nodes situated between each of the four corners. The shell element is computationally less expensive than both the solid elements previously listed making it an extremely valuable asset to a model that will be subjected to outof -plane bending forces. In order to create the optimal model, sometimes, as in the case of this research, it is necessary to incorporate multiple types of elements. When modeling with different elements it is of paramount importance that one realizes the limitations of each-creating the model to take advantage of the strengths of the element while limiting the influence of the weaknesses. 3.2 Initial Finite Element Models The finite element software used for this research was the ABAQUS program. This program was chosen due to the fact that there is more freedom in the creation of the model because it allows the user to choose the elements used in the meshing of the part. The Pro-Engineer program was initially used to model the fin, as this was the program used for the creation of the file used for the CNC in order to machine the mold. Once the geometry of the fin was created using the variable sweep extruding function in Pro-Engineer, the file was saved as a .stp file and exported into ABAQUS. It was in ABAQUS that the original meshing took place.

PAGE 47

47 3.2.1 The Completely 20-Node Hexahedral Mesh Initially it was thought that the automatic mesh generation tool in ABAQUS would be the best and easiest way to generate a successful model. The fin that was laid up for FEA verification was created solely from 45 degree plies. For this reason it was thought that the automatic mesh generator could be utilized and the fin could be modeled as being made out of a single anisotropic material. To create this model, the general stepby -step procedure in the program user interface panel was used. The steps taken to create the model are as follows: 1. The part was imported from the .stp file created in ProE. 2. A new material was created by using the material property manager and inputting the different values for the stiffness matrix of an anisotropic material. 3. A section was created that specifies the type of model desired. In this case a solid homogeneous section created from the material just specified. 4. The section and material properties were assigned to the imported part. 5. An instance of the fin was created for use in the application of loads and boundary conditions. 6. A step was made in which the actual loads would be applied. 7. The boundary conditions (clamped at the base) were specified. 8. The point load that was to be applied later experimentally was defined at the tip. 9. The mesh was generated using specified quadratic hexahedral elements. At the ninth step of the previous list the idea of creating the model from purely 20node came to a screeching halt. Since the geometry of the fin is so complex and the edges of the fin come together at such a small angle, the automatic mesh generator in ABAQUS failed to produce a mesh purely out of 20-node hexahedral elements. With this error message, the pure hex element approach was abandoned in search for another fast and easy solution.

PAGE 48

48 3.2.2 The Completely 10-Node Tetrahedral Mesh After the failure of the 20-node hexahedron mesh a similar approach as listed above was taken. The only difference in the second trial run of the creation of the model was the substitution of 10-node tetrahedral elements in lieu of the hexahedron. The geometry of the tetrahedron element is such that it was able to fit into the sharp edges of the fin geometry that the hexahedral elements could not. The same nine steps listed in section 3.2.1 were followed in this case but at the mesh step, the quadratic tetrahedron element was specified. This time the automatic mesh generator was able to successfully mesh the part. After the mesh was created a job was formed in which the analysis took place. Once the analysis finished some results were able to be viewed as shown by Figure 3-3 Figure 3-3: Deformation of fin using purely tetrahedron mesh under a point load With the creation of a model that was actually able to produce some results, a mesh refining process was then required. The purpose of refining the mesh was basically to check to see if the deflection of the fin would converge to a single number when the element size decreased. The 10-node tetrahedron element is not the best element for portraying bending, so this verification wa s critical. Initially the average

PAGE 49

49 tetrahedron size was set to 0.5 inches. This value was incrementally decreased by 0.1 inches. The maximum deflections in the negative z-direction are shown in Table 31. Table 3-1: Maximum deflections of the fin with the decreasing tetrahedron size Tetrahedron Size Maximum w Deflection (in) 0.5 4.16 0.4 4.14 0.3 4.13 0.2 4.06 After the tetrahedron size dropped below 0.2 inches the mesh generator was no longer able to produce a mesh. Also of note is that the automatic mesh generator was only able to fit two tetrahedron elements through the thickness of the fin. Since the tetrahedron elements are not known for their ability to accurately describe bending, a mesh with more than two through the thickness elements was desired. When viewing Table 3-1, it is seen that the results have no particular inclination to converge to a single value. This was also a reason that the purely 10-node tetrahedron mesh was decided to be an inadequate tool for the research. With the ultimate failure of the automatic mesh generator, it was necessary to take a closer look at what the model should ultimately accomplish and the best (if not the easiest) way to create such a model. 3.3 Development of the Final Finite Element Model Once it was clearly seen that the fast easy way to create the model was inadequate, a more detailed approach was taken. In this method the matrix based computational program MatLab was used to create an input file to be read and recognized by ABAQUS for the analysis of the model. Before creating the input file, a few primary goals for the new model need ed to be determined.

PAGE 50

50 3.3.1 Important Characteristics of the New Finite Element Model The failure of the automated mesh generator put a few problems in perspective and allowed for further specifications for the final finite element model. The following aspects were listed as characteristics that the final model should contain upon completion: 1. The model should utilize elements that c an accurately capture the bending/twisting characteristics of the fin. 2. The model needs to incorporate certain objects that can be easily changed once completed in order to make optimization easy. 3. The model needs to be created with ample number of elements through the thickness for more accurate deformation calculations. 4. Upon completion the model should be user friendly so that a person unfamiliar with the input file creation can use it as a design tool. With these objectives in mind, the creation of the .inp file was initiated. 3.3.2 Creation of an Input File Using MatLab When ABAQUS is used to analyze a model, before the job is submitted for analysis, an input file is created. This input file is basically an .inp file that states the nodes and their geometric position, element type and number, nodes associated with each element, interactions between nodes, material properties, boundary conditions, and loads. Depending on the geometry of the specimen and the type of elements used, the input file can be either extremely simple and short or very lengthy and complex. In the instance of this research the latter was definitely true. This section of the paper will allow the reader to catch a glimpse of the general process used to create the input file for the creation of the ultimate finite element model. The first step in the creation of the input file was the simple process of writing the necessary header required by all .inp files used in the ABAQUS program. After this was

PAGE 51

51 accomplished the fin geometry was setup in the program. To create the fin geometry, two different equations defining both the sweep of the leading edge of the fin and the complex airfoil shape of the fin were needed. To obtain these equations, the ProEngineer program was used to extract 23 nodal positions along the airfoil outer edge. After the 23 points used in the spline creation of the airfoil were found, these points were input into Microsoft Excel, and a tenth order polynomial was fit to the curve. The definition of the leading edge sweep was found by determining the major and minor radii of the ellipse and the radius of the circle at the tip that were used to control the position of the leading edge. The thickness profile as well as the leading edge curve can be seen in Figure 3-4 and Figure 35. Figure 34: Excel graph showing the thickness profile of the airfoil and the polynomial fit line

PAGE 52

52 Figure 3-5: Excel graph displaying the leading and trailing edge profiles Once the geometries of the fin were determined by equations, these equations were placed into the MatLab file. Before going any further it is necessary to state that the directions assumed in this research are a right handed coordinate system as follows: X-Direction starts at the root of the fin and points down the length Y-Direction starts at the trailing edge and points toward the leading edge Z-Direction starts at the mid plane and is assumed positive upward After the geometry of the fin was clearly defined, position points were defined down the span and chord and through the thickness of the fin. This was done by realizing that the thickness of the fin varies proportionally to the chord (y-direction) width and scaling the thickness of the fin accordingly Every step listed from this point on in this section will not be explained in detail for the fear that the paper would become hundreds of pages long. The commands associated with each step can be found in the ABAQUS User Manuel [14].

PAGE 53

53 Once the position of every point along the surface of the fin was found, node numbers were assigned to specific positions on and inside the fin. After the nodes were numbered and the positions defined, the element type to be associated with those nodes was determined. Using the element generation command, each element was connected to the required number of nodes (10 for tetrahedron, 20 for hexahedral, and 8 for shell). The type of elements used in the model and their locations will be described in the following sections. Surfaces (faces of certain elements) and edges were then defined for each element set. After each node w as included in an element, the interaction between different elements was defined. Specifically, elements that do not share nodes must be connected in some way so that stresses/strains can be transmitted from element set to el ement set. Element interactions can include the tying of two nodes together, the fixing of displacement between two nodes, and so on. Interactions are defined through placing interaction conditions between two of the surfaces previously created. Upon the completion of the interaction specifications it was necessary to create a material coordinate system for each set of elements. This was done by specifying certain nodes that should lie on the x-y-z or 1-2-3 coordinate system axes. Sections were then created for each element. The elements ha ving already been numbered must have certain properties assigned to each. This was done through the creation of sections. A section definition includes what type of section (solid or shell) will be used, the material property associated to that section, and the material orientation of that particular element set. Finally the material properties were defined by inputting the values of the stiffness matrix for the material of interest (graphite/epoxy). The next step

PAGE 54

54 in the process was the definition of the boundary conditions, and the nodes which were confined to behave as stated in each condition. The load was then input into the code with the corresponding nodes on which the load acted. The input file was then re ady to be imported into ABAQUS and run. Now that the creation of the MatLab input file has been reviewed it is necessary to look at exactly what elements were used and what features of the code were automated to achieve the previously listed goals for the model. 3.3.3 Shell Elements Utilized In order to attain the best bending and twisting characteristics in the model, it was decided that shell elements should be used. As stated previously in the introduction section, shell elements have an extremely accurate ability to portray bending. The first element sets created in the model were nine shell element sets. The shell sets created are as follows: 1. Two outer shells establishing the surface of the fin traveling from the root of the fin (x=0) to the tip of the fin (x=27.5 in.) 2. Two shells created so that the outer surface of these shells meshed up with the inner surface of the outer shells-these shells begin at the root and terminate at the specified end of the ply (initial case x=16.5 in.) 3. Two shells formed directly beneath the second set of shells with their outer -beginning at the root and ending at the end of the ply (initially x=11 in.) 4. Two shells made with the outer surface of these shells matching up with the inner surface of the third set of shells-beginning at the root and ending at the end of the ply (initially x=5 in.) 5. One mid-plane shell with no curvature traveling the length of the fin from x=0 to x=27.5 in. Each of these shells has a material coordinate system associated to each line of elements in the x-direction which can be viewed in Figure 3-6. The material coordinate

PAGE 55

55 system for each is important because every system has an out of plane axis normal to the surface of the shell. This was required to accurately assign material properties to each row of elements. Figure 3-6: ABAQUS rendering of the fin with only the shell elements created and each row of elements having own coordinate system As seen in Figure 3-6 each shell was accurately placed to represent one of the layers of graphite/epoxy used to lay-up the fin. It was chosen to create four shells on either side of the mid-plane because it is the lay-up and length of each of these layers that will be changed in the design process to make a better fin. The mid-plane shell was created for this reason as well, although the material orientation of the fabric will be the only change in this layer. With the nine shell element sets the bending and twisting characteristics of the fin will be more accurate. 3.3.4 Solid Elements Utilized Although the outer surfaces of the fin were taken care of through the use of shell elements, the inner portion of the shells cannot be left empty. For this reason solid elements were employed in the model. The inner layers of the fin will not be varied in the design process. These layers will all be uniformly laid up 45 degree

PAGE 56

56 graphite/epoxy material. For this reason distinct shell elements did not need to be created for every ply in the fin. The insides of the fin in the model were filled with a slew of solid elements including primarily 20-node hexahedral elements with the 10-node tetrahedral elements thrown in the model when their geometry was needed to fill space. A total of eight separate solid element sets were created to fill the voids left in the fin. Eight element sets were needed because of the use of drop-plies in the production of the fin. Four sets were situated on either side of the mid-plane shell. The first upper and lower set starts at the root and travels the length of the first drop-ply where they stop. The next two sets are thicker than the first two by the thickness of the first drop-ply. They start at the termination of the first drop-ply and end where the second drop-ply ends. The following upper and lower set is thicker than their respective predecessors by the thickness of the second drop-ply. These sets travel the span of where the second ply drops off to where the third drop-ply ends. The final pair of solid element sets fills the remaining space in between the outer shells and the midplane shells after the third drop-ply terminates. An example of how the thickness of each solid element set steps out can be seen in Figure 3-7 with Figure 3-8 showing all of the solid element sets in the model.

PAGE 57

57 Figure 3-7: Picture showing the width change in the solid elements at the termination of a drop-ply Figure 3-8: Picture showing each of the solid element sets with their respective material coordinate systems As with the shell element sets, each solid element row in a set was designated a coordinate system so as to properly assign material properties. Mentioned before was the use of both hexahedral and tetrahedron elements. It can be seen in Figure 3-8 that the 20-node brick elements (rectangular looking blocks in the middle) make up the vast majority of the solid element inner structure. The tetrahedral elements are used to fit inside the corner where the outer shells meet with the mid-plane shell. It takes three tetrahedron elements to fill the space of one hexahedral element. With the inclusion of

PAGE 58

58 the solid elements, the entirety of the volume within the outermost shell of the fin was filled with elements capable of accurately and precisely depicting the deformation of the fin under any loading condition. 3.3.5 Element Set Interactions and Boundary Conditions After all of the elements were created their interaction with each other was defined. Each element in a set is connected to similar elements in the same set due to the fact that adjacent elements share nodes. Because of this stresses are transmitted from one element to the next through the shared node. For elements in different sets, no common node exists through which stresses or displacements can be transmitted, for which reason node or surface interactions must exist. In the final model only a single interaction type was used, the tie interaction. The tie constraint was applied to the various element surfaces throughout the fin model. This constraint works in the following way. Two surfaces are defined, one on one element set and another on an adjacent element set. A master surface is specified as well as a slave surface. The master surface is responsible for transmitting the load to the slave surface. By tying the slave surface to the master surface, the load experienced by a node on the master surface is translated to a node on the slave surface that lies within a specified distance of the master node. Through the use of the tie constraint, a load applied on the outer surface of the fin will be experienced in varying degrees by all of the separate element sets and the deformations will be portrayed accurately. The following ties were applied: 1. The inside surface of the outermost shell master to the top surface of the outer drop-ply shell 2. The bottom surface of the outer drop-ply shell master to the top surface of the middle drop-ply shell

PAGE 59

59 3. The bottom surface of the middle drop-ply shell master to the top surface of the innermost drop-ply shell 4. The bottom surface of the innermost shell master to the top surface of the first solid element set 5. The bottom surface of the middle drop-ply shell master to the top surface of the second solid element set 6. The bottom surface of the outermost drop-ply shell master to the top surface of the third solid element set 7. The inside surface of the outer shell master to the top surface of the fourth solid element set 8. The bottom of solid element sets 1-4 master to the mid-plane shell top surface 9. The mid-plane shell bottom surface master to the bottom of the solid element sets 5-8 10. The inner surface of the shells 5-8 master to top surface of solid elements 5-8 11. Master-slave combinations for the shell sets on the bottom half of the mid-plane shell are mirrors of the combinations from the top 12. The back of the first solid element set master to the front of the second solid element set 13. The back of the second solid element set master to the front of the third solid element set 14. The back of the third solid set master to the front of the fourth solid set. 15. Front and back surface solid element ties mirrored from the top half of the fin to the bottom half of the fin These ties will make sure that the stresses are transmitted in the proper fashion through the fin. The next step was to create boundary conditions in the model. In real-life application, the root of the windsurfing fin is clamped inside of a windsurfing board. For this reason, a cantilever type boundary condition was applied to the model. This was the only type of boundary condition required in this model as it is the only motion

PAGE 60

60 constraint provided to the fin by an outside source. To accurately model this boundary condition, all of the nodes located on the x=0 y=0 plane were constrained. The nodes were constrained in all 6 degrees of freedom. Namely, the translational displacement in the x-y-z directions were all set equal to zero. The rotation about the x-y-z axes were also all set to equal zero. By doing this the root of the fin was effectively constrained creating the modeling equivalent of the real-life boundary condition. A cross section of the final model taken at the root of the fin can be viewed in Figure 39. Figure 3-9: Cross section of the final model illustrating all of the outer shells and the inner solid elements 3.3.6 Automated Design Features of the Final Model To create a model employing all of the previously listed theory and steps is all well and good if one has an excess amount of time on their hands. However, this model was created with the goal of saving time by eliminating the need of creating a new model every time a new fin was created. For this reason the model developed in this research has a few features built in to make it more of a design tool to the fin producer. The first design feature is the ability for one to change the material properties of the fin. When the MatLab code is initiated the user is prompted to input values for E 1

PAGE 61

61 E 2 E 3 12 13 23 G 12 G 23 and G 13 With these properties the stiffness matrix is calculated and the values automatically input into the correct portion of the code. The next special aspect of the code is the variability of the length of the dropplies. Similar to the material properties, the user is asked to specify values for the length of each drop-ply. Upon doing so, the code automatically adjusts the length of the shell elements used as drop-plies and also the solid element sets that fill the voids underneath those plies. The third and final design feature built into the code comes as the ability of the user to vary the fiber orientation of each ply as well as in the solid elements. It was stated before that each element set has a specific coordinate system associated with every row (line of elements along the x-axis) in that set. When initiated, after the MatLab code asks the user to specify material properties and ply length, it will prompt the user to enter a rotation of the fibers around the outof -plane (3) axis. Once a number is entered, the program will rotate the material properties of the element in the counterclockwise fashion so that each element in that set will act as if it were made from the material oriented in that direction. For example if 45 degrees is entered, the program will create a section and provide each element in that section with the material properties of the graphite cloth/epoxy rotated positive 45 degrees around the 3 axis. With the final adjustments to the code, a finite element model was created that not only will accurately describe the deformation characteristics of the fin laid up for use in this research, but will also allow the producer of the fins to play with a number of design factors to produce the best fin possible. The ABAQUS rendering of the final model can be seen in Figure 310.

PAGE 62

62 Figure 3-10: ABAQUS rendering of the final Finite Element Model

PAGE 63

63 CHAPTER 4 VISUAL IMAGE CORRELATION Every finite element model should be checked to make sure the computer generated results match up with experimental data. For problems involving simple beams, trusses, discs and other simple geometries, an analytical solution exists so that the computer model can be checked by a hand calculation. The high aspect ratio fin or airfoils with complicated geometries do not have these convenient analytical solutions. In the case of the fin, a different method for determining the real-life deformation characteristics must be utilized. For this purpose the visual image correlation (VIC) tool was used. 4.1 Background Information Visual image correlation is a common technique employed to measure the deformation of any object under an applied load. This method was initially created by researchers at USC and was originally referred to as Digital Image Correlation (DIC) n a region composed of a subset of pixels around a location where deformations are computed The VIC system is basically a pair of cameras setup in a triangular fashion with the sample. The cameras both take a photograph of a specially prepared specimen in an unloaded (reference) condition. Then, once the loads are applied, the cameras each take another photograph of the deformed specimen. After both the reference picture and deformed picture are taken, VIC computer software program is able to recognize specific areas spaced across the sample (discussed later on during the specimen preparation section). The software then takes all of the points located on the surface of

PAGE 64

64 the sample and compares the location of the spot on the deformed picture to the location of that same spot on the reference photograph. By doing this, a calculation is able to be made that will give the user the deformation of the sample. The VIC testing method is a full-field measurement technique capable of giving deformation information across the entire field of view shared by the two cameras. That being said it is important to pick the proper camera lenses to use for each specific test. Though capable of giving strain measurements, the VIC was only used for deformation information in this research. 4.2 Cantilever Point Load Test The first test that was performed using the VIC is a simple test where the bending characteristics of the fin were studied. To perform this test a point load was applied to the tip of the fin that was clamped at the root end. Before actually performing the test, a number of preparation steps were first followed. 4.2.1 Sample Preparation The initial step that was taken to prepare for the actual VIC test was the preparation of the sample. This step was critical in the grand scheme of the test, as it was th is process that enabled the cameras and computer software to make their measurements. To prepare the sample for the test, the fin that was laid up for the experimental testing to verify the FEA analysis was used. One of the surfaces of the fin was required to have randomly placed, easily identifiable, features on it so that the VIC software could spot these features to compare them between pictures and measure deflection (see Figure 41) To create these features on the surface of the fin spray paint was utilized. The spray paint steps are listed below. 1. One side of the fin was covered in a light coat of white spray paint.

PAGE 65

65 2. The paint was allowed to dry and then a second coat was sprayed on the same surface so that no dark areas of the underlying graphite fibers were showing. 3. While the second coat was drying, a pin was inserted into the spray nozzle of a black can of spray paint and wiggled around to widen the opening. 4. The black spray paint was then sprayed with the nozzle angled at around a 45 degree angle from the surface of a cardboard sheet of paper. 5. When spraying the black spray paint the nozzle was not fully depressed, but only partly so that the paint more sputters out than sprays. 6. The size of the paint speckles was examined on the cardboard paper checking for proper speckle size (the smaller the specimen the smaller the speckle size). 7. Typically a single speckle should be around three pixels by three pixels in size. 8. Once the speckle size was properly adjusted the same process for creating the speckle pattern is repeated over the entire white surface of the fin. 9. Upon completion of the black spot spraying, about half of the total area of the fin should be white background while half should be black speckles. Figure 4-1: Speckle pattern on a portion of the fin After the surface of the fin was prepared through the speckling process it was officially ready to be tested with the VIC system. 4.2.2 Initial VIC Test SetUp Before the VIC could be used to take the pictures, the proper experimental setup need ed to be arranged. Since it was desired to run a test that only bends the fin it was

PAGE 66

66 necessary to create a cantilevered type boundary condition for the fin. The first condition of this boundary constraint was that a rigid unmovable base be found to which the fin might be clamped. To satisfy this, the Newport PL-2000 Series Laminar Flow Isolator base was used with the Newport RP Reliance Sealed Hole Table Top attached to it. Though not expected to be any sort of a factor in the results obtained, the test was carried out on the bottom floor of the building eliminating any false readings that might theoretically arise due to excessive building vibrations. Another requirement of the base was that it must provide a means for clamping the fin. The Reliance Sealed Hole Table Top has quarter inch threaded holes set into the surface of the table spaced every inch. These made the base surface ideal for any sort of clamping needs. Next the fin need ed to be rigidly clamped to the unmovable base as seen in Figure 4-2. For this, a 7x2x2 inch piece of aluminum with two holes set through the thickness was used. When the fin was laid up in the mold, it was made longer than the modeled 27.5 inches long. The fin was ma de like this so that when the root of the fin was clamped in the windsurfing board only 27.5 inches of the fin was exposed. To accurately capture this in the VIC test, the forward edge of the strip of aluminum was placed on a line drawn perpendicular to the trailing edge, 27.5 inches from the tip of the fin. The aluminum was then screwed into the table top to secure the root of the fin. The trailing edge was lined up with the laminated tile lines on the ground to provide a reference position from which the cameras could be setup

PAGE 67

67 Figure 4-2: Picture showing the fin setup for the initial VIC test With the fin securely clamped the cameras then need ed to be positioned. Ideally, the cameras should make an equilateral triangle with the specimen to be tested. To make this possible a very wide variety of lenses need to be available to the tester. Since the fin is significantly larger than many of the wings and rotor blades tested at the University of Florida, the lens necessary to allow for the equilateral spacing of the cameras was not available. The lenses providing the largest depth of field were used (42 mm) Using these lenses and an adjustable leg length tripod, the cameras were set up so that the full length of the fin was included in the field of view of both cameras. The schematic of the set-up may be seen in Figure 43.

PAGE 68

68 Figure 4-3: Schematic of the VIC camera setup With the cameras set up with the fin in the field of view of both, the apertures or light exposure to each camera need ed to be adjusted. On the computer screen displaying the pictures of both fins, little red dots appear everywhere on surfaces that reflect too much light. Once the apertures were adjusted so that no red dots appeared on the length of the fin, any red dots displayed on any other surface (for example the shiny floor) were eliminated by a non-reflecting object (brown paper) placed over it to prevent reflections into the camera as in Figure 4-2. The fin and cameras were then fully prepared for the testing procedure. For complete instructions on the VIC testing 4.2.3 Initial VIC Test The first step in the actual testing procedure was the calibration of the VIC cameras. To calibrate the cameras a dot-matrix image paper need ed to be produced. The dot-matrix is basically a black background with uniformly sized white dots spaced evenly over it in a grid like pattern. Three of the white dots have smaller black dots at their center. The grid dot size varies between different dot-matrix image papers. A

PAGE 69

69 paper with dots on it whose size roughly match the size of the black speckles on the testing specimen was chosen. With the correct dot-matrix image paper in hand the VIC camera system was calibrated. To calibrate the camera system, the grid was placed as close to the surface of the fin as possible as seen in Figure 4-4. After positioning the paper at the root of the fin, a picture was taken using the VicSnap program. The grid was then moved incrementally down the length of the fin, changing the rotation of the grid at every location, and a picture taken at each step. The goal of the calibration picture taking process was to take in the ballpark of 20 photographs. It was also important to make sure that the dot-matrix image paper stay ed in the field of view of both cameras throughout the calibration photograph session. Once at least 20 pictures were taken with the matrix paper having covered the entire span of the fin, the cameras were ready for calibration. Figure 4-4: VIC image of the calibration process To calibrate the cameras, the Vic3D program was used. Inside the program it is possible to import all of the calibration photographs previously taken. Along with the

PAGE 70

70 importation of the calibration images, it was important to specify the dot-matrix grid pattern used for calibration. Each grid is specified by the number of white dots in the xdirection and y-direction, the spacing of the center of each white circle, and the offse t (number of points) between the white dots with the black dot in the middle. It was also the pictures imported, and the calibration grid and camera type selected the Vic3D was commanded to extract the calibration images. When the calibration images were extracted each picture was then viewed. If the cameras recognized the dot-matrix image then the white dots were filled in with color and the white dots with the black centers were a separate color. Once the images in which the grid was not recognized were discarded the software was able to calibrate each camera and calculate the standard deviations for the camera. The deviations were checked to insure accurate results and the cameras were officially calibrated. With the system calibrated the actual test was carried out. To perform the test, The VicSnap program was used once more. Once the program was initiated a reference photograph showing the fin in the unloaded condition was taken. Then weights were systematically hung from the tip of the fin using a very small clamp attached to the tip of the fin and loaded with weights hooked onto a string. Once the first weight is hung, as viewed in Figure 4-5, a few different pictures were taken so that at the end of the experiment the measured displacements can be averaged eliminating vibrations in the fin resulting from the application of the weight will be nullified.

PAGE 71

71 Figure 4-5: Image showing the application of the point load at the tip of the fin Six different loads were applied to the fin and at least three pictures taken for each loading scenario. At each load, a ruler was used to measure the tip deflection of the fin to help verify the computer results that will be obtained. After all of the loads were applied to the tip of the fin, the weights were recorded for future use and the Vic3D program was once again opened. With the calibration images still in the program the deformed images were imported into the program for analysis. In the program the reference image was selected and the area of interest defined for that image. The area of interest is basically a polygon created around the perimeter of the fin defining the area for which the user would like data to be calculated. Once the area of interest was defined a seed point was located to insure that the cameras are in correlation. The seed point is an easily identifiable speckle on the surface of the fin. Once the seed point was chosen on the reference image each of the cameras displays that point. If the point shown by both of the cameras matched the point selected then the image was accepted. The program then tried to find that point on all of the deformed images as well. Once successful in doing so, the analysis program was run.

PAGE 72

72 The analysis portion of the program found all of the spots on the fin in the reference image and correlated them to the same spots on the fin in the deformed images. Then the displacement values were calculated. The final step in the VIC analysis was the refining of the area of interest. After the deformation images have all been analyzed, the area that was actually studied could be reviewed. If the area did polygon perimeter was stretched and if too much area was covered it was shrunk. With the final fine tuning of the area of interest and the recalculation of the displacements by the program, the initial VIC test was completed. After the VIC analysis the deformation data was exported to a text file. Using MatLab, a deformation curve (Figure 4-6) was plotted for each of the loading conditions. The deformation curve was analyzed to make sure the computer data accurately represent ed the desired experimental conditions. Figure 4-6: Graph showing deformation of fin in the initial VIC test

PAGE 73

73 Upon viewing the graph depicted in Figure 4-5 a couple of observations, both good and bad, c an be made. First it is comforting to find that the tip deflection correspond ed well with the previously measured tip deflection roughly measured with a ruler. The unsettling part of the experimental data is the sharp decline depicted at the root of the fin. This sharp decline is indicative of an imperfectly applied boundary condition. In a perfectly cantilevered experiment, the slope of the line at the root of the fin should be zero at the very base and gradually build up to the maximum slope at the point of load. From looking at Figure 4-5 this is obviously not the case, making a few adjustments to the test necessary. 4.2.4 Modifications to Initial Test and Final VIC Test After looking at the deflection curve from the first test it was obvious that something had to be done to strengthen the boundary condition of the fin for an accurate test to be conducted. To this end, the clamped root of the fin was thoroughly studied under the bending loads applied in the first experiment. This study revealed that the flat undersurface of the rectangular bar of aluminum did not make full contact with the entire curved surface of the fin, and the flat table surface obviously also failed in similar fashion. While the boundary condition prevented the fin from lifting off the surface of the table, the clamp was inadequately formed for preventing the fin fro m rotating on the surface of the table. To fix the boundary issue stated in the previous paragraph it was clear that a rectangular base and a better clamping plate needed to be manufacture for the fin. Thankfully the solution to these problems was easily obtained. To create the rectangular base for the fin, a thin box was created out of Plexiglas with the top of the box left open. The root of the fin was placed in the open end of the box and the tip

PAGE 74

74 pointed skyward. The fin was made straight and level and bound to a wall to keep it from moving. Once secured, the West Systems epoxy used to lay up the fin was mixed with glass fibers and poured in the box to the line that marked 27.5 inches length from the tip of the fin. Glass fibers were used to increase the rigidity of the epoxy once cured. The epoxy was then allowed to cure over 24 hours before the box was broken away leaving the fin with a newly formed, ultra-rigid rectangular base perfect for clamping between two flat surfaces. To create a better clamp, a half inch thick piece of steel that was wider and longer than the base of the fin was used. Four holes were milled through the thickness of the steel through which screws could be placed. The fin was then placed back on the rigid table top and using four quarter inch screws, and a lot of torsion force, securely fastened. With the newly constructed base for the fin and clamp, the VIC experimental procedures listed in the previous section were once again performed. The results of this test can be viewed in Figure 4-6. When looking at this deformation curve it becomes obvious what a proper cantilevered boundary condition should look like. The slope at the base of the fin is zero and the fin deflection bends until maximum slope is obtained at the tip of the fin where the load has been applied. This successfully completed the bending test using the VIC.

PAGE 75

75 Figure 4-7: Results of using a rectangular based fin and stronger clamping condition for the VIC bend test 4.3 Twist Test Using VIC Although one experiment has been performed to check the computer-simulated to the real-life deflections of the fin, another was needed. The bend test is wonderful for determining if the computer model has the same bend characteristics as the real fin, but unfortunately there is more than bending to the actual deflection characteristics of a windsurfing fin. The other primary mode of deformation of a windsurfing fin or any airfoil is twist. Twist here is defined as the angle between two points having the same xposition on the fin but one lying on the leading edge, and one on the trailing edge. In order to accurately portray the deformation of a windsurfing fin, not only must the bending characteristics of the computer model match those of the experiment, but the twist deflections must match as well.

PAGE 76

76 4.3.1 Specimen Preparation For the twist test, the same fin laid-up for the sole purpose of this research design verification was used. Because of the recycled use of this fin, it was unnecessary to go through the entire gauntlet of sample prep used in the previous test. The surface was already speckled from the previous step and the base of the fin still securely rooted in the chopped fiberglass/epoxy rigid base. The only additional sample preparation that need ed to be performed for this test was developing a means to apply the torsion load to the fin. To apply torsion to the fin, a load sitting off of the surface of the fin need ed to be set. The initial thought was to use clamps to secure a rigid metal bar to the tip of the fin, perpendicular to the straight trailing edge. However, knowledge from the previous test showed the futility of trying to clamp a curved surface to a flat surface and obtaining reasonable test data. The solution to the clamping situation lied in the creation of a flat rectangular base of the tip of the fin seen in Figure 4-8, as was done for the root. Although the theory was similar a slightly different approach was taken for the creation of the tip box. Since a load was to be applied to the rectangular section of material attached to the tip of the fin, a more rigid material needed to be used to insure that the box material transmitted the torsion load as perfectly as possible to the fin. For this reason, a slot one inch deep and wide enough for the first inch of the fin tip to fit in was milled out of a thin piece of aluminum.

PAGE 77

77 Figure 4-8: Pro-Engineer rendering of the fin tip box Once this slot was created, two quarter inch holes were drilled through the thickness of the aluminum on either side of the slot. After the piece of aluminum was machined, the one inch tip of the fin was securely wrapped in a layer of Teflon sheeting and slid into the slot designated for it. The tip was wrapped in Teflon to allow the fin to release from the box after the test was administered. Next, the top edge of the aluminum was oriented as perfectly as possible so that it made a 90 degree angle with the straight trailing edge of the fin. Then, with the root of the fin this time pointing skyward and fastened to the wall, the small amount of epoxy necessary to fill the gap left between the aluminum walls and the fin tip was prepared and poured into the cavity. After 24 hours the epoxy cured and the fin tip has a very rigid rectangular section able to transmit the torsion load to the fin. This modification to the fin was the only necessary sample preparation in addition to what had already been done. 4.3.2 Twist Test SetUp The s et -up for the twist test progress ed in much the same way as the bend test and so will not be discussed in depth. The fin was once again clamped to the rigid table top using the steel slab machined for the previous test with the trailing edge lined up with the tile lines on the floor. The cameras were positioned and the apertures adjusted

PAGE 78

78 so that no red dots appear ed on the screen that included the full length of the fin in the field of view of each camera. The step in the test set-up not included in the previous test is preparing the fin for the application of the torsion load. To do this, a 25 inch long metal bar was connected by means of placing two bolts placed through the two holes in the aluminum box and bar with nuts fastened to the bolts to clamp the bar in place as seen in Figure 4-9. The bar was positioned at 90 degrees to the trailing edge so that the entire load was made to twist the fin. Figure 4-9: Fin set-up with torsion bar on tip of fin 4.3.3 Twist Test Procedure As with both the sample preparation and test set-up portion of this section, not much procedure changed between the test methods used for the bending test and the twisting test. The same dot grid was once again used to calibrate the cameras, the images extracted and the standard deviations calculated to insure they are sufficiently small (less than 0.07). The reference picture was once again taken. After the reference picture was taken, the bar was loaded by placing weights on the end of the bar. The center of the spot where the weights were applied was marked so that the exact

PAGE 79

79 distance of the load from the fin was able to be determined, and thus the moment calculated accurately. Several pictures were taken for three different loading conditions. At the conclusion of the loading portion of the experiment, Vic3D was once again used to make sure the cameras were properly distinguishing the different speckles on the surface. The area of interest was formed once more and the deflections of the fin obtained. With this, the entire experimental portion of the research was concluded, leaving only the cross checking computer data with experimental data and the fluid structure interaction portion of the research remaining. The results of the VIC tests will be shown in Chapter 5.

PAGE 80

80 CHAPTER 5 RESULTS AND DISCUSSI ON Before the final step of using the model created in the early stages of the research to obtain the real-life deflection characteristics of the fin, the experimental results must be analyzed. This chapter will look at the results from the mechanical testing, VIC experiments, and ABAQUS simulation. The results will also be discussed along with the possible influence of errors for each test. 5.1 Mechanical Properties Testing The first step taken in the research was the mechanical properties tests. As was stated in that chapter, two different tests were performed for this research-the tension test and the Iosipescu test. From these tests, values for the Modulus of Elasticity in the 1 and 2 directions (E 1 and E 2 ) were obtained as well as the Poisson Ratio in the 12 direction 12 ) along with the Shear Modulus in the 12 direction (G 12 ). 5.1.1 Tension Test Results Before any tests were made on the sample for the graphite/epoxy material used in the creation of the windsurfing fin, a piece of aluminum was tested. If the modulus of elasticity of aluminum could not be obtained to any degree of accuracy using the same strain gages that will be used to test the carbon fiber samples, the results cannot be trusted. To this end a 1x.26 inch cross section piece of aluminum was tested using the same testing machine and strain gages listed in the mechanical testing section of the paper. The results are seen in Figure 51.

PAGE 81

81 Figure 5-1: Stress Strain curve for aluminum sample The results of the aluminum tension test will be discussed in the following section. Suffice to say that the aluminum test yielded accurate enough results to continue the tests on the carbon fiber samples. Three samples were tested to help ensure accuracy of the results. The plots of all three of these samples are shown in Figure 5-2.

PAGE 82

82 Figure 5-2: Stress-Strain plot of all three graphite/epoxy sample The above figure will give values for E 1 and E 2 for the graphite/epoxy samples. However, this was only half of the information needed from this test. The uniaxia l 12 The following two tables show sample data for two of the three specimens (the third is not shown as the data acquired from this test was unreliable). Using Equation (1) and the data in Table 5-1 and Table 52 the values for the Poisson Ratio was found. Table 5-1: Sample values for Poisson Ratio from first sample Stress (Pa) Avg Strain 1 Avg Strain 2 12 3.81E+04 0.00131 5.64E 05 0.0428 4.37E+04 0.00148 6.58E 05 0.0443 4.80E +04 0.00161 7.27E 05 0.0450 5.12E+04 0.00170 7.78E 05 0.0455 5.28E+04 0.00175 8.09E 05 0.0461 5.44E+04 0.00179 8.24E 05 0.0457 5.47E+04 0.00180 8.08E 05 0.0447

PAGE 83

83 Table 5-2: Sample values for Poisson Ratio from second sample Stress (psi) Avg Strain 1 A vg Strain 2 12 23813.98383 0.000883 3.32E 05 0.0376 25716.78199 0.000948 3.75E 05 0.0395 26768.9476 0.000982 3.94E 05 0.0401 28801.28608 0.001051 4.28E 05 0.0407 30130.00629 0.001096 4.44E 05 0.0404 32720.34668 0.001183 5.07E 05 0.0428 34873.37201 0.001255 5. 49E 05 0.0436 5.1.2 Tension Test Discussion and Error After careful review of the data presented in the previous section, a few observations should be made. Initially, the data showing the modulus of aluminum needed to be investigated. From the graph and the line fit through the data, the tension test on aluminum yield ed a result for the Modulus of Elasticity of 9,738,744 psi or around 67.14 MPa. According to the website Engineering Toolbox [19] the modulus of aluminum, depending on its alloy and production method, ranges from 8.7 to 11.1 Msi. The value that was obtained from the uniaxial tension test lies comfortably between these two values making the test to ensure the testing equipment and strain gages function properly a success. Now that the ex perimental validation was performed, the graphs depicting the were studied. From the first, second, and third tests, the results are as follows: Test 1 E 1 = E 2 = 32.2 GPa Test 2 E 1 = E 2 = 27.89 GPa Test 3 E 1 = E 2 = 26.21 GPa

PAGE 84

84 The average from all three of these values lies somewhere around 28 GPa. These values were obtained by fitting a linear curve through the graphed data and finding the slope of that linear curve Although all three tests were carried out under precisely the same testing conditions there is some variance in the data. The error in the test data could possibly be a result of any of the following: 1. The strain gages on each sample were not perfectly oriented along the fibers in the samples 2. Though machined from the same plate, the fibers in each sample were not precisely aligned in one as they were in another (possibly a result from the fibers dragging during the hand lay-up process) 3. Different number of voids in the material of each sample 4. The cross sectional area measurement could have been off as a result of human error 5. Resistance of the dummy gage did not precisely match that of the strain gage because a 120 ohm resistor (not an unstrained strain gage from the same gage packet) was connected to the NI SCXI 1312 Any one or a combination of the four reasons listed above could have led to the spread in the data from the three uniaxial tension tests. Next, the data showing information concerning the Poisson ratio is examined. 12 is found for every stress-strain measurement. Taking an average of all of these readings the Poisson ratio was found to be as follows: Test 1 12 = 0.044 Test 2 12 = 0.040 The third test did not yield reliable data 12 is around .042. The reasons for error are speculated to be caused by the error for the measurements of E 1 and E 2

PAGE 85

85 5.1.3 Shear Test Results With the completion of the tension test results yielding values for four of the properties that were obtained during this research, it was necessary to examine the results of the second type of test performed. The shear test used the shear strain gages (see Chapter 2) mounted on Iosipescu samples and tested in the Iosipescu testing apparatus created at the University of Florida under the supervision of Professor Peter Ifju. This test gave data necessary for the calculation of the shear modulus G 12 The first test performed, as with the uniaxial tension test, was on an aluminum sample for which the data is shown in Figure 5-3. The purpose of this was once again to make sure the modulus for aluminum could be obtained with a certain degree of accuracy. Figure 5-3: Graph showing data for shear modulus calculations for aluminum After a brief examination of the data from the aluminum sample it is decided that the experiment was adequate to proceed with the data acquisition for a number of

PAGE 86

86 graphite/epoxy tests samples. The data from all of these samples are shown in Figure 54, the results of which will be discussed directly afterward. Figure 5-4: Plot showing data for shear modulus calculations for all three Iosipescu samples 5.1.4 Shear Test Discussion and Error Upon looking at the first aluminum shear stress shear strain curve, the slope (and thus the shear modulus) was observed to be close to 21 GPa. This value is slightly off of the quoted value of 26 GPa [19], but is still close enough to consider accurate. Error in the aluminum measurement may come in a couple of different forms. As was mentioned in the introduction to the shear testing section, the shear test was not as easily performed as the tension test, making the results by nature more various. Also, though the same strain gage was used for the aluminum test as was for the graphite/epoxy tests, the gages were not freshly mounted, decreasing the effectiveness

PAGE 87

87 of the bond and also potentially introducing error into the aluminum shear modulus calculation. When the plots for the three shear tests were viewed, and the slopes of the linear portion of the data calculated, the following results were obtained: Test 1 G 12 = 2.663 GPa Test 2 G 12 = 2.187 GPa Test 3 G 12 = 4.124 GPa When viewing these results, it is noted that the third test yields a modulus around 70 percent larger than the first two tests. It is now necessary to look at where error may have been introduced into these experiments. The majority of the error in this experiment can come from the bonding of the strain gage to the sample. As was stated in Chapter Two, the shear strain gage operates by taking the average of an uneven strain field developed in the Iosipescu test. If the strain gage does not cover the whole of the area between the notches, the strain measurements could be off. Another way error could be introduced was by not lining up the strain gage perfectly so that the vertical wires in the strain gage line up perfectly with the center of hole drilled into the specimen to make the notches. Other error sources include the application of inadequate gripping force by the Iosipescu test fixture so the specimen could slip. The improper alignment of the specimen in the apparatus so that the force when mounted in the testing machine is not in line with the notches in the specimen was also a source for error As with the tension test specimen, the measurement of the cross sectional area could have had human error associated with it. The specimens themselves could have been different as was stated in the tension test error section.

PAGE 88

88 With these sources for error the variance in the data was likely, but the idea of the mechanical properties testing was to get a ball park range for the material properties for the graphite/epoxy system used for the windsurfing fin. These properties were later refined during their input into the finite element code. Now that G 12 was obtained the data from the VIC should be displayed. 5.2 VIC Results The visual image correlation data was a very important part of this research. The data from both the bending and twisting tests were used for the ultimate verification of the model for the windsurfing fin. This portion of the chapter will look at the data obtained from both of the VIC tests to make sure the data appears sound. 5.2.1 VIC Cantilevered Bending Test The first tests from which the results were examined are the bending tests. For this experiment six different loading conditions were applied and data collected for each condition. For brevity, the deformation results will be shown for only one picture (Figure 5-5) of the six loading conditions, but the maximum deformation information will be listed for every test in Table 5-3 Also deformation information along a line on the fin will be shown for three loading conditions in Figure 5-6 to give a better idea of how the wdeformation changes from case to case. All of the dimensions in Figure 59 are given in millimeters.

PAGE 89

89 Figure 5-5: Deformations in the z direction of the fin under a 2.5 pound point load at the tip Figure 5-6: VIC W-Deformation vs. X-Position for three loading conditions (2.5, 6.5, and 11.8 pounds) Figure 5-6 makes intuitive sense. It shows that with increased load, the root obviously remain ed firmly clamped with zero deflection and increas ed deflections at the tip. The change in tip deflection was greater than the change in the mid-span deflection

PAGE 90

90 of the fin which also makes sense since there are more layers of graphite fabric in the mid-span of the fin, thus making that section less compliant. One interesting value that was studied is the maximum deflection at the tip for each picture; to make sure there is not too much variance between pictures. This data can be seen in Table 53. Table 5-3: Numerical results for maximum deflection of the fin at the six separate loading conditions Deformation Picture Load (lbs) Max W Deflection (mm) Max W Deflection (in) 0 0 0.00 0.00 1 0 0.27 0.01 2 0 0.14 0.01 3 0 0.18 0.01 4 2.5625 21.00 0.83 5 2.5625 20.86 0.82 6 2.5625 21.01 0.83 7 2.5625 20.95 0.82 16 3.875 30.66 1.21 17 3.875 30.45 1.20 18 3.875 30.49 1.20 19 3.875 30.69 1.21 20 6.4375 49.78 1.96 21 6.4375 49.80 1.96 22 6.4375 49.72 1.96 23 6.4375 49.78 1.96 8 9.25 67.60 2.66 9 9.25 67.70 2.67 10 9.25 68.52 2.70 11 9 .25 68.59 2.70 12 11.8125 87.86 3.46 13 11.8125 87.76 3.46 14 11.8125 88.02 3.47 15 11.8125 87.81 3.46 After looking at the maximum deflection at the tip of the fin (where vibrations due to the addition of the weights are greatest) it is seen that the variance in data from one

PAGE 91

91 picture to the next in a specified loading condition was negligible. Because the deformation data taken over the area of the complete fin and the maximum deflection data from the tip of the fin all correlate well to the test, the results were deemed worthy of this research. 5.2.2 VIC Twist Test The next VIC test that was integral in verifying the model was the twist test. For the twist test three separate loads were placed at the end of the bar responsible for creating the twisting moment on the tip of the fin. Three pictures were taken at each of these loads. As with the bending test, only one deformation picture will be shown for the three tests, as seen by Figure 57. Also Figure 5-8 will show the varying twist for two of the load cases (the jagged data will be corrected in the following sections). The maximum twist values at the tip will be listed in Table 5-4 for each of the pictures taken at each of the three different loads. The values of each graph are given in inches. Figure 5-7: Picture showing the deformation of the fin when 5.8 pounds are applied to the bar

PAGE 92

92 Figure 5-8: VIC twist calculations for two separate loading conditions (5.8 and 8 pounds) Table 5-4: Numerical results for the maximum twist at the tip of the fin under a variety of torsion loading conditions Picture Load (lbs) Max Twist at Tip (radians) Max Twist at Tip (degrees) 1 0 0 0 8 5.8125 0.0442 2.53 9 5.8125 0.0444 2.54 10 5.8125 0.0445 2.55 2 6 0.0464 2.65 3 6 0.0465 2.66 4 6 0.0457 2.62 5 8 0.0625 3.58 6 8 0.0620 3.55 7 8 0.0613 3.51 From looking at the previous table it can be seen that the change in the maximum twist at the tip, and thus the twist at any point in the fin was minimal in comparison to

PAGE 93

93 the change in w-deformations undergone during the bending tests. Also, vibrations between pictures were negligible. Larger loads were not applied to keep the bending of the fin at a minimum as the observation of the twisting characteristics of the fin was the main objective of this experiment. With the conclusion of the VIC testing, it is now necessary to apply the same loads to the finite element model to check the deformations and hopefully match them with the experimental data. 5.3 ABAQUS Results Now the VIC testing was performed and the data stored and analyzed. T he ABAQUS model was then run with simulated loads that very closely replicated the experimental tests. This section outlines the results of those tests. 5.3.1 ABAQUS Cantilevered Bending Test The first test to be run in the FEA software was the simple cantilevered bending test. To simulate this loading condition a point load equal to the weight of the clamp and the applied weights was placed on the tip of the fin (in the same location as in the VIC experiment). An analysis was performed for each of the loading conditions, but only the results for the medium load (6.5 pounds) will be displayed in Figure 5-9. As with the VIC data three deformation curves will also be displayed in Figure 5-10. For each of the loading conditions, the same material properties were input into the code. These properties were obtained from the mechanical testing. The properties unable to be determined by this method were found in a literature search [1,2] and by using the rule of mixtures. They can be seen in Table 55.

PAGE 94

94 Table 5-5: Material Properties input into the final FEA code Material Property Value (psi) Value (GPa) E_1 4351132 29.99 E_2 4351132 29.99 E_3 750000 5.17 v_12 0. 042 0.042 v_13 0.248 0.248 v_23 0.248 0.248 G_12 435000 2.99 G_13 300000 2.06 G_23 300000 2.06 Figure 5-9: Medium load deformations as modeled in ABAQUS

PAGE 95

95 Figure 5-10: ABAQUS W-Deformation vs. X-Position for three separate loading conditions (2.5, 6.5, and 11.8 pounds) 5.3.2 ABAQUS Twist Test The twist test was the next and final test to be modeled by the model developed for this research. For this test the same material properties were applied as in the bend test in the previous section. The sole difference between the two tests was the applied load. The load that was applied for the twist test was both a moment and a point load. Each of these loading conditions was placed on a node on the surface of the fin corresponding to the position on which the actual load acted during the VIC tests (the geometric center of the bar in the x-direction but the mass center of the tip of the fin in the y-directions). The point load was equal to the total weight of the bar and the applied weights, and the moment consists of the weight of each mass (bar and applied weights) multiplied by the distance from which it acts (see Figure 5-11) One of the loading

PAGE 96

96 condition results, the case with a larger applied weight (eight pounds), will be shown in Figure 5-12 with two twist curves being shown in Figure 513. Figure 5-11: Schematic illustrating forces experienced by the fin under twist load Figure 5-12 : ABAQUS deformations under large applied torque

PAGE 97

97 Figure 5-13: ABAQUS Twist deformation curves for two separate loading conditions (5.8 and 8 pounds) 5.4 Matching the Data from ABAQUS and VIC Now that all of the data, both computer and experimental, was gathered it was important that a method be devised for performing a more rigorous comparison between the two sets of deflection data. It was this comparison that ultimately determin ed whether or not the model accurately capture d the deformation characteristics of the windsurfing fin. The data is shown in this section. 5.4.1 Matching the Bend Test Data The first method that was developed for more accurately comparing the deflection data was created for the bending tests. In order to make this comparison possible a node path was created in ABAQUS for which the y-position is constant and the xposition varies from the root to the tip of the fin. The node path was chosen to hold a yposition of approximately one inch from the trailing edge of the fin. The w-deflections

PAGE 98

98 for each of the nodes along this path were easily found in ABAQUS by specifying such as the field output. Once the x-position and w-deflection of every node were found, they were input into an Excel file. MatLab was then used to find the position of data points in the VIC deformation .txt file that correspond closely with those retrieved from ABAQUS. Namely, all of the data points with a y-position of around one were chosen and their respective x-positions and w-deflections recorded. These recorded values were then placed with the ABAQUS values in the Excel file. Using the spreadsheet, a scatter plot was created showing the deformation curve of both the VIC and ABAQUS data. A third order polynomial was fit to these curves and the R-squared value recorded along with the equation of the line. Finally, x-position values were specified from 0-27.5 inches in increments of half of an inch and the deflection values were calculated for each. Using these values an error measurement was made and an average error of the deflection curve found. This comparison was performed for the small, medium, and large loading conditions for which the deformations were shown in the previous section and the results follow in Figure 5-14 and Table 5-6.

PAGE 99

99 Figure 5-14: Deflection curves comparison for three loading conditions Table 5-6: Equations of the fit lines and R-squared values for three loading conditions Load (lbs) Polynomial Fit Curve (ABAQUS) R^2 Value (ABAQUS) Polynomial Fit Curve (VIC) R^2 Value (VIC) 2.5 y = 1.6778E 05x 3 5.0760E 04x 2 5.6999E 04x + 6.8918E 04 R = 9.9997E 01 y = 1.2391E 05x 3 7.1798E 04x 2 + 1.2966E 03x + 1.2640E 03 R = 9.998 6E 01 6.5 y = 3.8223E 05x 3 1.2490E 03x 2 1.0507E 03x + 1.2200E 03 R = 9.9997E 01 y = 3.3417E 05x 3 1.5351E 03x 2 1.0539E 03x + 7.7835E 03 R = 9.9996E 01 11.8 y = 5.8858E 05x 3 2.3022E 03x 2 6.1765E 04x + 3.8129E 04 R = 9.9997E 01 y = 4.5275 E 05x 3 3.2642E 03x 2 + 4.9185E 03x 3.5107E 03 R = 9.9999E 01

PAGE 100

100 Using the equations for the third order polynomials given in Table 5-6, the average error of the deflection curves is found. They range from 3.5 percent for the 2.5 pound loading condition to nine percent for the 11.8 pound loading condition. Since this is under ten percent it is deemed acceptable. 5.4.2 Matching the Twist Test Data With the successful matching of the bending test data it was necessary to see if the data sets for the twist test also matched. This was the test of primary importance because, as implied by the application of a point load and a moment in the model, the fin will bend and twist under the twist test loading conditions. Therefore not only was the twist measured and compared but the bend curves of the fin also were compared in the step. As with the bend test, a method for comparison was developed for the twist test. In order to measure the twist of the fin in ABAQUS, two more node paths were developed in the same manner as the bend test. Instead of the node paths being one inch from the trailing edge of the fin however, one of these node paths was inset from the trailing edge by a half of an inch and one inset from the leading edge by a half of an inch. For each of these node paths the x-position, y-position, and w-deflections were found by specifying each in the field output of the ABAQUS results window. The twist was then calculated by creating a right triangle out of the position and deformation points of the fin by the equation: (Equation 2) The twist for the VIC data was found in a similar way by using MatLab and finding points inset by a half inch off of the trailing edge. Then these x-position points were

PAGE 101

101 input into the equation defining the leading edge of the fin to obtain the exact y-position of a point inset a half of an inch from the leading edge corresponding to that x-position. In the same program, the points most closely corresponding to these leading edge points were found along with the values for the w-deflection associated with each point. Twist for each point was calculated using the Equation 2. The bend data from the twist deflection test was found using the exact method listed in the preceding section. With these sets of data an accurate comparison of both the bend and twist deformation characteristics can be made for both a small load torsion test (5.8 pounds applied) and a large load torsion test (8 pounds applied). As with the bend data, the deflection points were input into an Excel file and a polynomial fit to the data. Before going any further it is necessary to study Figure 5-15 which shows the extracted points from the VIC test. Figure 5-15: Plot showing the leading and trailing edge profiles obtained from ABAQUS and the VIC data

PAGE 102

102 Looking at the profiles for the leading and trailing edges, it is clearly seen that some of the VIC points (namely from 15 inches to 22 inches) along the leading edge of the fin d id not closely match the ABAQUS data. This result ed in th e jagged twist curves shown in Figure 5-8. For this reason in the comparison analysis some of the points were excluded from the deflection calculations to create the smooth deflection curve indicative of the actual experimental data. Now that the method was developed the data was analyzed and is viewed in Figure 516 and Table 5-7. Figure 516: Plot showing twist deformation comparison for two loading conditions

PAGE 103

103 Table 5-7: The fourth order polynomial and R-squared value of twist comparison for small loading case Load (lbs) Polynomial Fit Equation (ABAQUS) R^2 Value (ABAQUS) Polynomial Fit Equation (VIC) R^2 Value (VIC) 5.8 y = 1.5424E 05x 4 + 4.9497E 04x 3 6.8297E 03x 2 + 3.1524E 04x 1.5991E 02 R = 9.9969E 01 y = 1.4480E 05x 4 + 4.7550E 04x 3 6 .6213E 03x 2 + 4.7915E 04x 5.9977E 03 R = 9.9960E 01 8 y = 2.1731E 05x 4 + 6.9725E 04x 3 9.6316E 03x 2 + 2.9069E 04x 2.2813E 02 R = 9.9968E 01 y = 1.9088E 05x 4 + 5.9256E 04x 3 8.0544E 03x 2 3.3653E 03x 1.5740E 02 R = 9.9981E 01 It should be noted that for the twist comparison a fourth order polynomial was used as opposed to the third order polynomial used for the bending comparison. The Rsquared values matched up more perfectly without exception using a fourth order polynomial for the twist test and a third order polynomial for the bend comparison. Using these equations the error in the 5.8 pound load twist test is around five percent and less than ten percent for the eight pound load twist test. The bend data was analyzed for the two twist tests, the results of which are shown in Figure 517 and Table 5-8.

PAGE 104

104 Figure 517: Bend data comparison from the two separate loads twist tests Table 5-8: Third order polynomial and R-squared values for bend data from small load twist test Load (lbs) P olynomial Fit Curve (ABAQUS) R^2 Value (ABAQUS) Polynomial Fit Curve (VIC) R^2 Value (VIC) 5.8 y = 3.7484E 05x 3 8.5777E 04x 2 3.3107E 03x + 3.6281E 03 R = 9.9997E 01 y = 1.3932E 05x 3 1.2859E 03x 2 2.2710E 04x 3.1930E 03 R = 9.9999E 01 8 y = 1.8066E 05x 3 1.9321E 03x 2 2.1665E 03x 4.5032E 03 R = 9.9999E 01 y = 1.8021E 05x 3 1.9325E 03x 2 + 4.5349E 04x 4.5044E 03 R = 9.9999E 01

PAGE 105

105 Using the equation listed in Table 5-8 and x-values ranging from 0-27.5 inches, the average error in the bend data extracted from the 5.8 pound load twist test was near seven percent with the error for the 8 pound load twist test sitting at five percent. 5.4.3 Match ed Curves Discussion Now that the data for the w-deflection and twisting deformation curves has been presented it is necessary to review the data and discuss the results and some possible sources of error. When viewing the average error from the bend tests, it was seen that as the deflections increase the error between the two curves defining the deflections also increases slightly but stays under ten percent. Therefore, the error in between the ABAQUS and the VIC data is acceptable as it is always under ten percent. The twist test data also has error bounded inside the ten percent range. This error also increases as the loading conditions increase. As with the bend data, extremely large twisting conditions are not expected in real-life performance and so this data is deemed acceptable. Some sources of error were indeed present in this procedure. The first source of error included the imperfect application of the modeled load. The bending and loading conditions experienced by the fin for the VIC tests were modeled as a simple point load, and a point load and a moment respectively in ABAQUS. These modeled loading conditions may not have matched perfectly with the real-life loading conditions. Also, although great care was taken to insure otherwise it is definitely possible that human error was associated with the VIC experiments. For example, the bar used for the torsion test may not have been exactly oriented at 90 degrees with respect to the trailing edge, or the application of the point load in the bending test could have resulted in a moment created about the tip of the fin. Finally, the lay-up of the fin created for

PAGE 106

106 verification could differ slightly than the one modeled in ABAQUS. In the FEA program, an ideally created fin was modeled. This model assumes no voids and perfectly aligned fibers in the fin, which is not a completely perfect assumption but very difficult to correct. All in all though, the data obtained from the VIC and the model coincides nicely.

PAGE 107

107 CHAPTER 6 ATHENA VORTEX LATTICE METHOD With the successful matching of experimental and theoretical data obtained from the Visual Image Correlation and ABAQUS respectively, the deformations of the windsurfing fin under a real-life loading condition need ed to be determined. This was the last step in the research. Once the hydrodynamic loading conditions are applied to the fin in the non-deformed shape and the deformation characteristics are found, the model can become a design tool for the user to help maximize the performance of the fin by varying the ply orientation, drop-ply length, and materials used in the creation of the fin. In order to accurately capture the hydrodynamic forces experienced by the fin, the Athena Vortex Lattice program was used. 6.1 Background Information ortex Lattice (AVL) 1.0 was originally written by Harold Youngren circa 1988 for the MIT Athena TODOR aero software collection. A number of modifications have since been added by Mark Drela and Harold Youngren, to the point where only a aerodynamic forces on any airfoil structure along with some slender bodies such as the fuselage of an aircraft. The program works off of the creation of three input files. The first input file specifies the main geometry of the airfoil specifying the location of the required nodes and number of panels spanning the surface of the fin. The second input file gives the density of the fluid in which the airfoil will be acting along with the mass and inertia information of the airfoil. The third and final input file on which the program operates specifies the running conditions of the airfoil. Specifically this file gives the information pertaining to the velocity of the fin, the center of gravity of the fin, the

PAGE 108

108 reference span and chord length, the surface area of the airfoil, the angle of attack, and the coefficient of lift and drag. AVL then takes these inputs and outputs a discretized horseshoe vortex acting on the quarter chord of each panel. Once calculated by AVL it is then up to the user to create a method for distributing these vortices to the proper locations in their FEA model, for the accurate capturing of the aerodynamic loads. The AVL program can also be used to discover the hydrodynamic loads on a windsurfing fin. By changing the values for the density of the fluid in which the airfoil (or fin) acts, the program becomes a tool for calculating forces on a fin submerged in water rather than an airfoil in air. 6.2 Running AVL and Applying Loads to the Finite Element Model Before ABAQUS can be used to calculate real deflections on the undeformed fin under hydrodynamic loading conditions, it was necessary to make a few calculations for and modifications to the AVL program. For example, geometric properties needed to be determined. The changes and program use will be shown in the upcoming sections. 6.2.1 Running AVL Before AVL could be run, as was mentioned in the introduction section, a few properties of the fin need ed to be defined. To start out with, some geometrical characteristics of the fin were determined. The surface area of the wing and center of mass in the x/y/z-directions were found first. To calculate surface area the equation for the leading edge of the fin was used in integration from the root to the tip of the fin. The coordinate system for AVL is different than that used for the finite element model. The origin for this system lies along the mid-plane of the symmetric airfoil shape and at the intersection of the lines defining the root and trailing edge of the fin. The x-axis points downstream while the y-axis points down the span of the fin. Finally, the z-axis follows

PAGE 109

109 the right hand rule and is positive upward. For the location of the y-center of mass, Equation (3) was used where f(y) is the equation of the leading edge. Equation (3) To locate the center of mass in the x-direction Equation (4) was used. Once again f(y) is the equation of the leading edge of the fin. Equation (4) After the geometrical properties of the fin were defined, it was necessary to also state some of the operating conditions of the fin. The fin will be running in most scenarios in the ocean, so the viscosity and density of the fluid characteristics were set as such. Since the fin will experience a variety of angles of attack, the FEA simulation ran through several scenarios varying the AOA. Finally, the velocity and Mach number of the fin were determined. During a typical windsurfing race, the sailor and fin will experience velocities ranging from 10-30 knots (11.5-34.5 miles per hour). For this reason three different AVL loading scenarios were run, one for 10 knots, one for 20 and the final for 30 knots. The Mach number was found simply by dividing the speed experienced by the fin by the speed of sound in seawater. With the inputs set the MatLab program used to run the AVL program was initiated and the AVL program in turn produced a series of numbers corresponding to forces acting on the quarter chord of each panel of the specified geometry. To get a better feel for the forces experienced by the fin, Table 6-1 shows the net force acting on the fin for varying speed and angle of attack.

PAGE 110

110 Table 6-1: List of test data along with net force acting on the fin under each operating condition Experiment Number Velocity (m/s) Angle of attack (degrees) Ply Orientation (degrees) Net Force (lbs) 1 5.14 1 45 32 2 5.14 2 45 65 3 5.14 3 45 97 4 5.14 4 45 130 5 10.28 1 45 130 6 10.28 2 45 261 7 10.28 3 45 391 8 10.28 4 45 522 9 15.43 1 45 293 10 15.43 2 45 587 11 15.43 3 45 881 12 15.43 4 45 1175 Wh en looking at the data presented by Table 6-1, it is noticed that the forces experienced by the fin at high velocities and sharper angles of attack are extremely large especially considering that these forces are a result of a windsurfer leaning on his/her board and stressing the fin. To verify that the forces output by AVL were in the correct range, a back of the envelope calculation was performed to determine lift forces on a NACA airfoil closely resembling the cross section of the fin. In order to perform this calculation, Equation 5 was employed. Equation (5) In this equation C L is the coefficient of lift, is the density of the fluid, v is the speed at which the fin is traveling, and A is the surface area of the top surface of the fin This calculation was performed for the conditions listed in Table 6-1 and the results are shown in Table 62.

PAGE 111

111 Table 6-2: Net force experienced by NACA 0009 under given conditions Constants Density (kg/m^3) Area (m^2) 1025 0.07259 Angle of Attack ( degrees) Coefficient of Lift Velocity (knots) Velocity (m/s) Lift (N) Lift (lbs) 1 0.117 10 5.14 114 25 2 0.233 10 5.14 229 51 3 0.35 10 5.14 344 77 4 0.466 10 5.14 458 103 1 0.117 20 10.28 459 103 2 0.233 20 10.28 916 206 3 0.35 20 10.28 1376 309 4 0.466 20 10.28 1832 412 1 0.117 30 15.42 1034 232 2 0.233 30 15.42 2061 463 3 0.35 30 15.42 3096 696 4 0.466 30 15.42 4122 927 After comparing the net force results from the AVL calculator and the back of the envelope calculations, it was seen that the forces experienced by the fin are in the same range for both methods of calculation. For this reason the higher velocity scenarios were run at significantly smaller angles of attack. This gives a more accurate representation of the actual loading conditions in a typical windsurfing session. 6.2.2 Applying Loads to the Finite Element Model Now that the forces on the quarter chord of each of the pre-defined panels were found, these forces were applied to nodes in the actual finite element model. AVL requires that the span-wise spacing of the panels be uniform, and the model did not fit this requirement. For this reason a separate mesh (shown in Figure 61) still defining the surface area of the fin but with equal span-wise spacing, was created for the sole purpose of running the AVL program.

PAGE 112

112 Figure 6-1: MatLab graph rendering the fin surface input into the AVL program Once the analysis program was run, MatLab was used to find the exact location (x and y positions) to which each of the forces defined by AVL correspond. Since the airfoil shape of the fin is symmetric, AVL outputs forces acting on the plane of symmetry (z=0). For this reason, the nodes on the mid-plane shell with x and y positions that most closely corresponded to the positions of the AVL forces were found. The forces from AVL were then used along with their corresponding nodes from the finite element model to define the real-life loading condition in the input file used for the ABAQUS analysis which can be seen in Figure 6-2. With the real-life loading condition determined, ABAQUS was used for deformation analysis.

PAGE 113

113 Figure 6-2: ABAQUS rendering of the forces from AVL applied to the final finite element model 6.3 AVL Loading Condition Results and Discussion Once the finite element analysis of the complex loading condition of the fin was run, it as of interest to view how the fin deform ed at each of the three speeds (10, 20, and 30 knots) and variety of the angles of attack experienced throughout a typical windsurfing race. Also a few preliminary simulations were run to determine how the deformation of the fin varied when the orientation of the fibers in the fin were changed. To do this, the fiber orientations of all of the element sets in the model were set to 0 and 90 degrees. With a test run for every single one of these variable conditions, a total of twenty four tests were run. A sampling of the results follows in Figure 6-3.

PAGE 114

114 Figure 6-3: W-deflection of fin traveling 20 knots with one degree AOA and 45 degree ply orientation Only one ABAQUS deformation graph will be shown in this paper as the other graphs are almost exactly the same, with the single difference coming as the deflection values listed in the legend. Tables 6-3 and 6-4 show the maximum deflection of the fi n (which always occurs at the tip). Figure 6-4, 6-5, 6-6 show a few deflection curves for different action scenarios.

PAGE 115

115 Figure 6-4: Deflection curves for 10 knot speed and different angles of attack and ply orientation Figure 6-5: Deflection curves for 20 knot speed and different angles of attack and ply orientation

PAGE 116

116 Figure 6-6: Deflection curves for 30 knot speed and different angles of attack and ply orientation Table 6-3: List of maximum deflections for given loading scenarios for 5 ply or ientations Velocity (m/s) Angle of attack (degrees) Ply Orientation (degrees) Net Force (lbs) Maximum W Deflection (in) 5.14 0 45 0 0 5.14 1 45 32 1.83 5.14 2 45 65 3.66 5.1 4 3 45 97 5.49 5.14 4 45 130 7.32 10.2 8 0 45 0 0 10.28 0.75 45 97 5.49 10.2 8 1 45 130 7.32 10.28 1.25 45 163 9.15 10.28 1.5 45 195 10.9 15.43 0 45 0 0 15.43 0.1875 45 55 3.13 15.43 0.375 45 111 6.26 15.43 0.5625 45 164 9.22 15.43 0.75 45 220 12.36

PAGE 117

117 Table 6-4: Maximum deflections of 0/90 degree ply orientation at given loading scenarios Velocity (m/s) Angle of attack (degrees) Ply Orientation (degrees) Net Force (lbs) Maximum W Deflection (in) 5.14 0 45 0 0 5.14 1 0 32 0.70 5.14 2 0 65 1.40 5.14 3 0 97 2.10 5.1 4 4 0 130 2.80 10.28 0 0 0 0 10.28 0.75 0 97 2.10 10.28 1 0 130 2.80 10.28 1.25 0 163 3.51 10.28 1.5 0 195 4.21 15.43 0 0 0 0 15.43 0.1875 0 55 1.2 15.43 0.375 0 111 2.40 15.43 0.5625 0 164 3.53 15.43 0.75 0 220 4.73 Looking at the deflections of the fin in each of the four loading conditions, some conclusions may be drawn. First, it should be noticed that the maximum deflections increased rapidly with increas ed angle of attack. Looking at Table 6-1 this should come as no surprise as the sum of the forces acting on the fin in the z-direction also increased at an exceptional rate with the higher angles of attack. When viewing the bending curves of each fin it was noticed that most of the bending occurs at the root of the fin, This makes sense as the thickness and chord of the fin are much greater towards the root, thus making the bulk of the forces be concentrated there. Finally, the lay-up of the fin was seen to make a tremendous difference in the deformation characteristics of the fin. Looking at the three degree angle of attack scenario for the 5 degree and 0/90

PAGE 118

118 degree cases it was seen that the maximum deflection of the 5 fin was around two and a half times greater than the deflection of the 0/90 fin. This also makes sense as the fibers (when oriented at 0 and 90 degrees) were responsible for determining the deflection which result ed in a much stiffer fin. All in all, the results obtained from the AVL loading conditions make intuitive sense and verify that the model is completely capable of being used as a design tool for any production company.

PAGE 119

119 CHAPTER 7 CONCLUSIONS AND FUTURE WORK 7.1 Conclusions At the outset of this research, the ultimate goal of creating a design tool for the production of a high aspect ratio, variably swept, thin airfoil was stated. In order to accomplish said goal a windsurfing fin was created for verification purposes. Using the same production method as was used for the fin, test specimens were created to obtain data leading to the discovery of the material properties of the material. After receiving these properties, a variety of methods were evaluated to create a finite element model that had the ability to accurately capture the deflection characteristics of the fin. Also important in the design of this model was the ability of a user, not familiar with the creation of the model, to be able to use this model as a design tool by being able to easily manipulate input variables such as material orientation, drop-ply length, and material properties. Upon the successful creation of such a model, it was necessary to test the design tool through experimental verification. To this end a number of tests were performed using the Visual Image Correlation full-field experimental technique. The experimental deformation characteristics of the fin were then compared with those obtained through use of the finite element model created and tested in ABAQUS. Error analysis was performed for the different tests under a variety of loading conditions. At the conclusion of these tests it was decided that the error, though present, was well within the acceptable design range, and that the model was ready to undergo a loading condition that could be verified only by intuition, not experiment.

PAGE 120

120 The final step in this research was the use of the Athena Vortex Lattice program to determine the loads undergone by the fin during a typical windsurfing race. A variety of tests were run in AVL to obtain the loading conditions for a fin traveling at 10, 20, and 30 knots with angles of attack varying from .1875 to three degrees. After these deflection conditions were obtained using ABAQUS and the model, the fiber orientation was changed from the initial 5 degrees to 0/90 degrees and the tests run again. Through these tests it was ultimately determined that the finite element model was suited for the task of being used as a design tool to optimize the performance of the windsurfing fin used for design verification. After the successful completion of the various portions of this research, a finit e element model consisting of 8-node shell, 20-node hexahedral, and 10-node tetrahedron elements was found to accurately portray the deformation characteristics of a high aspect ratio, variably swept, thin airfoil under any loading condition. Though some error was present in the data, it was such that the effectiveness of this finite element model would not be compromised during its use as a design tool. For this reason the research was deemed a success. 7.2 Future Work Though the research was concluded successfully there remains some work to be done. If desired, further tests using the VIC could be performed to obtain more verification of the model. More tests could also be run, modifying the material properties of the fin input into the model to more completely eliminate error in the bend and twist curves of the VIC and finite element model data. Finally, work still stands to be done in the optimization of the fin. In order to perform this optimization one would have to play around with the variables in the code (ply orientation, drop-ply length, and

PAGE 121

121 material properties) to create a fin which contains the perfect amount of bend and twist under realistic loading conditions.

PAGE 122

122 LIST OF REFERENCES [1] Daniel, Issac M., Luo, JyiComposites Part B Feb. 2007: 14. [2] Hyer, Michael W. Stress Analysis of Fiber-Reinforced Composite Materials New York: McGraw Hill, 1997. [3] Murray, William M., Miller, William R. The Bonded Electrical Resistance Strain Gage: An Introduction New York: Oxford University Press, 1992. Micro-Measurements, 2006. [5] "Omega.com". Omega Measurements and Control Products. 01/20/10 . [6] "Determining the Ultimate Tensile Strength of a Composite Material". Nanopedia. 01/20/10 . [7] "Tensioning Webs: Web Mechanics". WebHandling.com. 01/20/10 . -Measurements Strain Gage with M-Bond 200 and AE-10 Micro-Measurements, 2008. Journal of Materials 2(3): 537-566. Jornal of Composite Materials Aug. 1991: 26. [13] "Volume Meshing Commands". Fluent Incorporated. 01/24/10 . [15] Sankar, Bhavani V., Kim, Nam-Ho. Introduction to Finite Element Analysis and Design New York: John Wiley and Sons Inc., 2009. Implementation of a SecondExperimental Mechanics Dec. 2000: 393-400.

PAGE 123

123 [17] Peters, WH. and Ranson, WE, "Digital Imaging Techniques in Experimental Stress Analysis," Opt. Eng. May 1982: 21,427-432. Florida. 2006. [19] "Young Modulus of Elasticity for Metals and Alloys". Engineering Tool Box. 02/02/10 . 2006.

PAGE 124

124 BIOGRAPHICAL SKETCH Jarrod Bonsmann first came to the University of Florida from Lake Mary High School in Orlando, Florida in the fall of 2004. Initially a physics major, after two semesters he determined that his future lay in a different direction. His fascination with all things flight related made the change to aerospace engineering an easy an obvious decision. Eight semesters after beginning at UF, Jarrod graduated with his Bachelor of Science in aerospace engineering from that very same university. During his undergraduate career, Jarrod had a few different opportunities to learn from Professor Peter Ifju and upon graduation decided that with consent he would continue his education under that same professor. Two years and loads of knowledge later, Jarrod graduated from the University of Florida with his Master of Science degree in mechanical engineering. While at UF, during all six of his calendar years there.